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model up

model up
Question 1:
Undertake the Roller bracket exercise as detailed in section 3 of the Tutorial exercise book. You will need to create part models of all the components that make up the Roller Bracket device as well as the Roller Bracket assembly model.
Also create a simple detail engineering drawing of the Base part. For this drawing you are required to show appropriate orthographic views, with dimensions, and a 3D view. You do not have to include tolerances and surface finishes but you should include a drawing sheet border and a completed title block.
Question 2:
Figure 1 depicts a foot-operated pump commonly used for inflating pneumatic tyres. The drawings that follow are for the various components making up the pump. The drawings are not reproduced to the same scale and some drawings are not fully dimensioned.
The pump could be provided with one of two different pressure gauges – one having a Ø50 mm body and the other a Ø60 mm body. It is desirable to have a clearance gap of 3 mm between the gauge and the cylinder, see figure 1, irrespective of what gauge is used. To accomplish this you need to set up a parametric relationship between the gauge body and the dimension marked with * in the Fitting drawing of figure 5. Now, if the gauge body dimension is changed then the * dimension of the Fitting is automatically updated and the 3 mm gap between the gauge and cylinder is maintained.
The Project
Your task is to model up the various pump components and the assembled pump. More specifically you are required to:
1. Create parametric feature-based solid models for all the components, either shown or listed in the following pages.
2. Create an assembly model showing all parts in their working position when the return Spring is compressed to an overall length of 44 mm and the pump is fitted with the Ø50 Pressure gauge.
3. Set up a parametric relationship between the Pressure gauge and its Fitting that will preserve the 3 mm gap as described in the background section above.
Guidance on the Project
You will be expected to combine some research with sound practical judgement to obtain missing details in the information given and the drawings provided.
Before commencing this assignment you should think about the function of each feature and each part and how the individual components might be made. Also consider the physical assembly process i.e. how the parts actually fit together and the order in which the components might be put together. Your model creation process should reflect this wherever possible. Some guidance is given in the instructions for the Roller Bracket exercise.
The flexible hose does not have to be modelled. The Pressure gauge and the piston Valve models need only be representative of their physical shape and size as shown in the drawings provided.
What and how you need to submit
Your assignment is to be submitted in a compressed (zipped) folder for each question .
For question 1, submit one compressed folder with:
• Electronic copies of all the Creo3.0 models – i.e. part ‘.prt’ files and assembly ‘.asm’ files*
• An electronic copy of a ‘.pdf ‘ file for the Base drawing.
• An electronic copy of an A4 sheet (in .pdf format created from a word document) with a listing of the file names you used for each part and each assembly.
For question 2, submit one compressed folder with:
• Electronic copies of all the Creo3.0 models – i.e. part ‘.prt’ files and assembly ‘.asm’ files*
• An electronic copy of an A4 sheet (in .pdf format created from a word document) with:
A listing of the file names you used for each part and each assembly and
Instructions on how to ‘test’ the parametric relationships between the Pressure gauge and its Fitting.
Check that all files, in particular the assembly files, open correctly from your compressed folder before submitting it. It is very important that you do this as a marks penalty will apply if the files cannot be readily accessed by the markers.
*If you use a program other than PTC Creo3.0 parametric you will need to convert your files to Creo ‘.prt’ and ‘.asm’ files. If your software does not support this conversion then save or export them as IGES or STEP files. Either way you should also submit all original / native model files – e.g. if you use Solid Edge then you would need to submit the Solid Edge files as well as the IGES or STEP files. You must also include screenshots (in ‘.pdf ‘ format) of the model / feature tree directories so that your model creation process can be assessed. Submit all these files in a single compressed folder for each question. You will also need to include a detailed account of how you set up the parametric relationship and how to test it.
Figure 1: Foot-operated pump
Figure 2: Pump details
Figure 3: Pump details
Figure 4: Pump details
Figure 5: Pump details
Figure 6: Pump details
Exercise 2 – parts and assembly
Module 3 – Exercise 2 – parts and assembly 3.1
3.1 Roller Roller bracket example bracket example
In this tutorial, we will create the five parts that comprise the Roller bracket shown in the detail drawings of figure 3.1. Each part will be developed in Creo3.0 parametric. All parts will then be assembled together as shown in figure 3.2.
You should have already completed the Box part tutorial and be fully conversant with the instructions used to develop this part. Do not attempt the following exercise if you have not completed the previous exercise.
In this tutorial, basic instruction is given and, in many cases, you are expected to determine the precise key strokes and menu commands as required.
We will now start to concentrate on some of the ways in which the design intention can be captured in the part development. As a general rule, keep each feature fairly simple and keep adding features until the basic part shape is complete; then apply new features that pertain to the most likely manufacturing processes.
Figure 3.1: Roller bracket details
(Source: Boundy, AW. 2007, Engineering drawing, 7th edn, McGraw –Hill, Sydney, p. 241.)
Module 3 – Exercise 2 – parts and assembly 3.2
Figure 3.2: Roller bracket assembly model
3.2 Setup
You should have already created a sub-directory folder for this project called Roller_Bracket. If not do it now – refer to section 2.2.2.
Start Creo3.0 and set the working directory through File> Manage Session>Select Working Directory navigating to the Roller_Bracket folder – OK. Each time you open up Creo to work on the Roller_Bracket project you must set the working directory to this folder. This will ensure all your model and drawing files are in the one location.
3.3 Part development: bracket
Figure 3.3: The bracket
Foot feature
Module 3 – Exercise 2 – parts and assembly 3.3
3.3.1 Before you start
It is a good idea if you bookmark page 3.1 because you will need to refer to figure 3.1 frequently. Better still, have your text by Boundy opened at page 256 so you don’t have to flick back through these pages.
One of the main requirements of the cast bracket, also in figure 3.3, is that it is symmetric about its centre plane. It is also clear that the hole sizes and spacing must relate in some way to those dimensions on the Base part (item 2). Let us begin.
Create a new part called Bracket (item1) and select mmns units. Remember this is one component of the Roller bracket assembly.
Now switch off the display of Coordinate Systems and Spin Centre. We do not need them or want them visible in any of the printouts that may be required later on.
3.3.2 Creating the bracket foot
The foot of the Bracket (i.e. the bottom feature of component 1) will be created as a one-sided solid extrusion sketched on the top plane.
Select the Sketch , then pick the TOP datum plane as the sketch plane, and reference the RIGHT datum plane so that its orientation is to the right side. Sketch to close the window. The RIGHT and FRONT datum planes now become References to measure from.
Hover the cursor over each of the drawing icons in the Sketching panel under the Sketch tab to re-familiarise yourself with their functions.
Sketch a Centreline (Sketching panel) on the TOP plane coincident with the RIGHT plane – i.e. on the reference line that intersection of the TOP and RIGHT datum planes – see figure 3.4. Your centreline should snap to the existing reference line.
click to exit the line draw mode.
Module 3 – Exercise 2 – parts and assembly 3.4
Figure 3.4: Creating a centreline
Now sketch one half of the bottom view of the bracket, with the bottom Line starting at the origin and drawn to the right coincident with the FRONT datum plane. Then draw a second line parallel to our centerline and finally a third line back to the centerline – as in figure 3.5. Make sure that the second line is not the same length as the first line and do not close this shape.
Figure 3.5: Initial sketch of bracket foot
button to cease line draw.
Sketch this centreline
Sketch this shape
Start here
RIGHT plane
TOP plane
FRONT plane
Module 3 – Exercise 2 – parts and assembly 3.5
Now create a Fillet (not an arc) in the top right corner. See figure 3.6.
Figure 3.6:Half the sketch of the bracket foot
You should see little greyed out dimensions appearing – these are the Intent Manager’s best guess of what the dimensions should be. We will tidy these up later.
Select all geometry by either
? from the Operations toolbar and then by holding down and clicking on each line
? from the Operations toolbar and then by placing a selection window over the sketch
? Choose All geometry from the expanded Select icon
Now choose Mirror (from the Editing ribbon panel) then select the vertical centerline that we created. Symmetry should now be ensured – figure 3.7.
Module 3 – Exercise 2 – parts and assembly 3.6
Figure 3.7: Mirrored view
Change the display to Sketch view and Refit – figure 3.8. The dimensioning scheme needs improving so that it conforms to the given drawing and the design intent.
Figure 3.8: The sketch view
Force a dimension between fillet centres by choosing the Normal dimension icon ; click on the left fillet centre; click on the right fillet centre, and click above the sketch to place the text. You should see a new dimension
Module 3 – Exercise 2 – parts and assembly 3.7
between the centres and the overall dimension should disappear. Force a vertical dimension from the bottom line to one of the fillet centres.
Choose the Select arrow . Now modify the values of the three dimensions to 12, 50 and 34, by double clicking on the text of each dimension in turn. The sketch regenerates after each change. The final sketch shape is shown in figure 3.9.
Figure 3.9: Dimensioning the foot sketch
OK to finish sketching. Now revert to the standard view display.
Select Extrude . Make sure the extrusion direction is pointing up from the top datum plane. If not then click on the directional arrow to change it.
Set the Dashboard depth Options to Blind (i.e. Extrude from sketch plane by a specified depth) and set the depth value to 10 – enter.
Green tick to complete the feature as shown in figure 3.10. Rename this feature.
Figure 3.10: The completed bracket foot
Module 3 – Exercise 2 – parts and assembly 3.8
3.3.3 Creating the boss
It may seem strange, but we will create the main boss section next. Turn off the datum plane display and deselect all features (move the cursor to a blank screen section and click.
Sketch on the front face of the existing feature (figure 3.11 insert). Set the underneath surface of the foot to the Bottom Orientation. Sketch button to close the window.
Change the display to Sketch view
Refer to figure 3.11. Sketch a circle lying in the middle of the part and above the top surface of the foot. Force a dimension from the bottom of the part to the centre of the circle. Modify the values to 62 and 32 (It is much better to use a 32 mm diameter rather than a 16mm radius in this instance). OK to exit sketcher.
? Set to Standard orientation
? Extrude
? Direct the extrusion rearwards
? Set the depth of the extrusion to 14
? Green Tick to complete the feature
? Rename the feature
See figure 3.11 for the sketch and partial model insert.
Figure 3.11: Bracket base and boss
Front face
Module 3 – Exercise 2 – parts and assembly 3.9
3.3.4 Creating the R5 front fillet
Because we are removing material here we cannot use the ‘round’ command. We need to create an extruded cut i.e. we need to ‘remove material’.
Sketch on the right face of the existing base – not the RIGHT datum plane – figure 3.12, first diagram. Set the upper face of the foot as the reference and orient this face to the Top. Sketch button to close the window.
Figure 3.12: Sketch face for foot R5 cut
Change the display to Sketch view and Hidden line – figure 3.13
Figure 3.13: Sketch of bracket foot R5 cut
Sketch face
Module 3 – Exercise 2 – parts and assembly 3.10
Sketch the R5 arc using the Centre and ends command as shown in the figure 3.13.
OK to complete the sketch.
Set to the Standard orientation and turn on Shading.
With the sketch selected Extrude this feature. Now direct the cut back through the foot. From the Dashboard – figure 3.14a set the following:
? Extrude as solid
? Remove Material
? Extrude to intersect with all surface
Solid Depth
Remove material
Figure 3.14: R5 cut in base
to build the feature. Rename it FRONT_FILLET.
3.3.5 Creating the boss support
Sketch on the back face of the circular protrusion i.e. the Boss. Select the upper face of the foot as the reference and choose Top as its orientation.
Close the Sketch window. Change the display to Sketch view and Hidden line – figure 3.15a. This is a rear view of the Bracket.
Open the References window (Setup tools) then select the outer edge of the circular boss as an additional reference. Close the References window.
Insert a horizontal Centerline through the Boss by first clicking on the boss centre and then clicking elsewhere so as to snap the centerline horizontally.
Module 3 – Exercise 2 – parts and assembly 3.11
Create a Rectangle , with its top left corner touching the left side of the circular protrusion and the bottom right corner touching the top of the lower feature as shown in figure 3.15. The sketch should be aligned and not require any dimensions. OK for done.
Set to the Standard orientation and turn on Shading.
Select Extrude . Direct the extrusion forward and set depth option to Extrude up to selected point, curve, plane or surface. Carefully the select the top edge of the R5 cut – figure 3.15, second diagram. Complete the feature . Rename the feature.
Figure 3.15: Bracket boss support
3.3.6 Creating the 10mm web
Display the datum planes.
Refer to figure 3.16 to create the web (the triangular gusset feature – sometimes called rib):
? Sketch tool
? Pick the RIGHT datum plane as the sketch plane and orient the upper face of the foot to the Top
? Sketch to close the Sketch window
? Change the display to Sketch view and Hidden line
? Open the References window (Setup tools) and add the back face of boss and rear face of foot as additional references – figure 3.16
? Close the References window
? Draw a diagonal Lineand dimension as shown in the first diagram of figure 3.16
select this corner first
Then select this corner
extrude up to this edge
Module 3 – Exercise 2 – parts and assembly 3.12
? OK to complete the sketch
? With the sketched line still highlighted select the Profile Rib tool from the Engineering panel
? Direct the arrow into the corner of the bracket – second diagram in figure 3.16
? Change web thickness to 10 mm
to complete feature
Dynamically rotate the model and turn the shading on. The completed feature should look similar to the last diagram in figure 3.16.
Figure 3.16: Bracket web
* Add these as references
Module 3 – Exercise 2 – parts and assembly 3.13
3.3.7 Creating R16 rounds, boss and base holes
Using the Round tool (Engineering panel) create the R16 rounds between the upright support and the base – figure 3.17.
Add a 12mm hole to the boss.
? Make sure the datum axes are displayed
? Choose the Hole tool
? click) the front face of the boss. This is the primary reference for the hole i.e. this is the surface to be drilled
? With down select the axis of the boss. The axis is a secondary reference and the hole is now coaxial with the boss axis
? Set diameter to 12
? Change the depth option to Drill up to next surface
? Complete the feature build
It would make sense to locate the 12 mm base holes so that their centres are coincident with the R12 round centres. To do this we are first going to create a datum axis that passes through the one of the rounds.
Choose the Axis tool (Datum panel) then select the R12 round curved surface – first diagram of figure 3.17. Creo will place the axis through the centre of this partial cylinder. OK the Datum axis window.
Using the same technique as creating the boss hole add a straight hole of diameter 12 that is coaxial with this datum axis and passes through the base.
To copy this hole:
? Select the Hole feature
? Mirror tool (Editing panel)
? Select the RIGHT plane ( you can select it from the Model tree if your datum planes are not displayed)
? Green tick
Module 3 – Exercise 2 – parts and assembly 3.14
Figure 3.17: R16 rounds and 12mm holes
3.3.8 Completing the bracket
Complete the part by creating rounds for the R5 fillets as shown in figure 3.18. Select multiple corners by holding down while clicking on each corner.
Figure 3.18: Complete bracket
Rename the features and Save the part.
Saving your work shouldn’t be an issue provided you have set the working directory correctly. Even so, you should always check the file path before saving. If you need to, refer back section 2.8.
R16 round
12 mm boss hole
12 mm base hole
Round surface
Module 3 – Exercise 2 – parts and assembly 3.15
3.4 Part development: base
3.4.1 Before you start
Refer to figure 3.19. The Base must be symmetric about two axes and the most important dimensions are the centre-centre distances between the holes – not the overall nominal dimensions. We need to dimension to the hole centres, but we cannot create the holes without first creating a solid feature. The Base would be cast with the 3 mm machining relief included, and the two shoulder sections would be machined. The dimension between the shoulders is relatively important as it provides location stops for the Brackets which we will see later in the assembly. This then really leaves the 46mm dimensions redundant. All four holes should be the same size.
Figure 3.19: The base
3.4.2 Creating the first feature of the base
If you have not already done so or this is a new session make sure that you Select your Working Directory to the same folder eg. Roller_Bracket where the Bracket part is filed.
Create a new part called Base.prt
The first feature for the Base model will be a sketched solid extrusion. Now, instead of creating the sketch first and then turning it into a feature, as previously done, we can initiate the feature building command and if that feature requires a sketch then it will be included as a step within the feature building process. This type of sketch is referred to as an internal sketch. Set the standard orientation and turn on the plane display. With this technique it is best to deselect all features before beginning.
Module 3 – Exercise 2 – parts and assembly 3.16
? Choose Extrude tool
? Select the TOP datum plane
This should take you into the sketch environment.
We are going to sketch one quarter of the Base section and then use the sketch mirror function to create the initial feature of whole Base.
? Insert two Centerlines (Sketching panel), one coincident with the RIGHT datum plane and one coincident with the FRONT datum plane – see figure 3.20
? In the far right quadrant, sketch two lines that represent the edges of the Base – see figure 3.20. Note, the sketch is on the TOP plane and I have hidden the other two planes for clarity.
Figure 3.20: One quadrant of the Base first feature
? Add a Fillet at the corner of the two sketched lines
? Select all geometry and then Mirror about one of the centrelines and then Select all geometry and this time Mirror about the other centerline
Arrange the dimensioning so that the three dimensions are the fillet radius and the two centre-centre distances. Now modify their values to 12, 50 and 134 – figure 3.21. (It may help to change to the Sketch view . This makes it easier to see the true geometry shape. Change back to the Standard orientation when the sketch is complete).
? OK to complete and exit sketcher
In the Dashboard extrude the feature as a solid to a depth of 14 above the top plane. Complete the feature . Refer to the second diagram in figure 3.21.
Sketch these centerlines
Module 3 – Exercise 2 – parts and assembly 3.17
Figure 3.21: Base first sketch and feature
If you expand the Extrude feature in the model tree directory you will note that the internal sketch is embedded as a subset of the feature. Previously, the sketch was a separate entity as well as being attached to the feature – figure 3.22.
Figure 3.22: Sketch comparison
Rename the feature.
3.4.3 Creating the machine relief
This will be another extruded feature using an internal sketch. However, we will remove material this time instead of adding material. Also we will select the sketching surface (only) before choosing the extrude command. Set the display to Standard orientation and deselect all features.
? Select the front face (not plane) of the existing feature as the Sketch plane
o To do this first select the model feature
o Now select the front face of this feature so that it is highlighted – see figure 3.23
Internal sketch
Unattached sketch
Module 3 – Exercise 2 – parts and assembly 3.18
Figure 3.23: Selecting the sketching face
? Choose Extrude
? Change the display to the Sketch view and No hidden
? Sketch a vertical Centerline (Sketching panel) – figure 3.24
You may want to turn off the datum display. Now sketch one half of the machining relief by first drawing a quadrant Arc using the Centre and End option – figure 3.24.
Figure 3.24: Sketching the side of the relief
Now draw a Line from the end of this arc to the vertical centre line. Mirror all geometry about the centreline of the Base. Force a dimension of 54 from one end as shown in figure 3.25. Force the depth dimension 3. (You may be alerted that the geometry is dimensionally over defined. If so, you will then need to delete one of the dimensions in the Resolve Sketch window. Pick the radius dimension and Delete it.)
Figure 3.25: Completed sketch of the machining relief
Sketched centreline
Module 3 – Exercise 2 – parts and assembly 3.19
? OK to exit Sketcher
? Set to standard orientation and shading on
? Redirect the extrusion through the Base
? From the Dashboard set
o Extrude as solid
o Extrude to intersect with all surfaces
o Remove material
? Now complete the feature
? Rename this feature
Figure 3.26: Base machining relief
Module 3 – Exercise 2 – parts and assembly 3.20
3.4.4 Creating the machined steps
These will also be internal sketched extruded features which remove material.
? Choose Extrude (make sure all features are deselected first)
? Select the front face (not plane) of the existing feature as the Sketch plane
? Change the display to the Sketch view and No hidden
? Open References (in the Setup panel). Click on the top edge and the left-hand vertical edge of the Base. This will add references which will assist sketching and also make later dimensioning easier. Close the References window.
? Sketch one of the machined shoulders i.e. one short vertical line and a horizontal line
? Sketch a vertical Centerline (Sketching panel) that is coincident with the mid-plane of the Base
Now we will add a dimension to represent the distance between the shoulders.
then click on the little vertical line you just drew, click on the vertical centreline, click on little vertical line again, and then click where you want the dimension placed. Add another dimension from the bottom of the Base to the height of the shoulder (obviously, we want to specify the minimum thickness of the shoulder for strength and assembly purposes). Modify these dimensions to the correct values of 66 and 12. See figure 3.27.
Figure 3.27: Base machine step
To add the 66 dimension
? select small line*
? select centerline
? select small line* again
? Position cursor to place the dimension – middle click
Module 3 – Exercise 2 – parts and assembly 3.21
? OK to exit Sketcher.
? Set to standard orientation and shading on
? Redirect the extrusion through the Base
? From the Dashboard set
o Extrude as solid
o Remove material
o Extrude to intersect with all surfaces
? Complete the feature – see figure 3.28
Figure 3.28: Base machined steps
In a large production run, we may use a specialist milling machine to cut both shoulders at the same time. If so, we could have made the sketch on the preceding cut include both shoulders. A better way is just to mirror the feature now (this is one of the rare times where mirroring a feature, (as opposed to a sketch, makes sense). Pick the shoulder feature, select the Mirror , pick RIGHT plane from the model tree, and complete the feature .
Figure 3.29: Base machined steps
Rename the feature
Module 3 – Exercise 2 – parts and assembly 3.22
3.4.5 Adding M10 holes
First create a datum axis through one 12mm round corners. (If you forget how to do this then refer to section 3.3.7 – about half way through this section)
To create a threaded hole:
? Create the datum axis
? Choose Hole
? Select the top face of the shoulder
? With pressed select the axis of the round
? In the Dashboard click Create standard hole -refer to figure 3.30 for hole settings)
? Set the thread type to ISO
? Set thread major diameter and pitch to M10 x 1.5
? Set the depth of the thread to Drill to intersect with all surfaces
? click on the Shape tab and turn on the Thru thread option
? Turn off both Countersink and Counterbore buttons if they are active
? Complete the feature
Figure 3.30: M10 hole settings
Thru Thread
Std hole
C’sink / C’bore option
Thread type
Thread size
Module 3 – Exercise 2 – parts and assembly 3.23
Mirror this hole about the relevant datum planes to create the other three holes.
You can view the thread details by selecting the hole, button down to display the pop-up menu and choose Edit Definition . From the Dashboard click on the Note tab. Refer to figure 3.31. This note identifies the thread as being metric (denoted by M); the pitch being 1.5 mm; the major diameter as 10 mm and the drill to create the minor diameter as 8.5 mm. This information can be added to a detail drawing of this part as a note if required.
to close the Dashboard.
Figure 3.31: Thread details
You can turn off the thread display details in the model through in the graphics toolbar.
If you zoom in and examine the model of the thread you will notice that the thread form (i.e. the helical groove) is not displayed. This is normal in Creo for Hole threads and cosmetic threads. However, the working drawing depiction of threads conforms to conventional drawing standard as will be seen later.
Turn off all datum displays and view the model in the No Hidden mode to see how the threaded holes are displayed. Refer to figure 3.32, first diagram.
Sometimes this thread root display can clutter the drawing and model. To hide this display, select the hole (or holes) and button down and choose Hide. See figure 3.32, second diagram. This procedure can be reversed to bring back the normal thread display if needed. Unhide the thread before moving on.
Figure 3.32: Wireframe display of threaded holes
Turn the shading back on – figure 3.33. Give the features more appropriate names before you Save the part .
Module 3 – Exercise 2 – parts and assembly 3.24
3.5 Part development: roller
3.5.1 Before you start
Refer to figure 3.34. The Roller is essentially cylindrical in shape. Also, it must be symmetric about its mid-plane. Therefore the length dimensions should be created symmetric to this mid-plane. All of the main dimensions are diameters, not radii – so make sure we capture this in the part. The Roller would be cast with its overall shape already defined. However, to make sketching and feature creation simpler, we will make the Roller without the centre hole and without the casting rounds. We will not make half a Roller and mirror this feature because we don’t make the Roller by welding two halves together. This time we will sketch a basic shape and revolve this shape around its central axis.
Figure 3.34: The roller
3.5.2 Creating the roller
If you have not already done so or this is a new session make sure that you Select your Working Directory to the same folder eg. Roller_Bracket where the Bracket and Base are parts are filed.
Create a new part called Roller.prt.
Display the datum planes and set to the standard orientation.
This is a revolved feature. Once again we will incorporate an internal sketch.
Mid plane
Revolve axis
Module 3 – Exercise 2 – parts and assembly 3.25
? Deselect all features
? Select Revolve tool from the Shapes panel
? Select the FRONT datum plane
Insert a horizontal Geometry Centreline from the Datum panel (not the Construction Centerline from the Sketching panel) that is coincident with the TOP and FRONT datum planes –this first centreline will always be the axis of revolution.
Now create a vertical Construction Centreline (Sketching panel) that is coincident with the RIGHT and FRONT datum planes – figure 3.35.
Figure 3.35: Inserting the centrelines
Change the display to the Sketch view and No hidden. Turn off the datum display.
Now sketch the upper right quadrant of the Roller similar to that shown in figure 3.36. When sketching this shape do not allow the intent manager to dictate all constraints. Sometimes it gets it wrong. For example, intent manager has a tendency of aligning lines and making lines the same length if your sketching objects are close to these constraints.
Do not close this shape.
Geometry Centreline
The sketch will be revolved about this
Construction Centreline
Module 3 – Exercise 2 – parts and assembly 3.26
Figure 3.36: Initial sketch for the roller
Mirror this sketch about the vertical centreline (that lies on the RIGHT datum plane).
We now need to apply a dimension arrangement similar to that shown in figure 3.34. At this stage do not be concerned about the actual dimension values. They can be corrected later. The automatically generated dimensions for my shape are shown in figure 3.37. Yours will most likely be different.
Figure 3.37: Initial sketch for the roller
Mirror centreline
Module 3 – Exercise 2 – parts and assembly 3.27
The dimensions displayed in figure 3.37 are sufficient to fully define the shape – otherwise Creo would show an error. However, you should notice some dimensions, mainly angular, have replaced certain linear dimensions given in figure 3.34. We need to force those linear (including the diameter) dimensions in our sketch.
Rearrange all the vertical dimensions so they appear as diameter dimensions. These dimensions need to be symmetrical about the axis of rotation.
? If you forget how to create these diameter dimensions…
o Choose the dimension tool
o click on the line or point to dimension
o click on the centerline
o click again on the line or point to dimension
o move the cursor to place the dimension value and click
Now arrange the depth (horizontal) linear dimensions. The mirror function will have ensured symmetry of these dimensions about the vertical centerline – which is what we want.
Finally, modify all the dimensions to their correct values – but be careful that you don’t make an impossible object!!! Start with the smallest dimensions first, otherwise the sketch may try to turn itself inside out. Your completed sketch with correct dimensioning should look like that in figure 3.38.
Figure 3.38: Dimensioning the roller sketch
Module 3 – Exercise 2 – parts and assembly 3.28
? Exit sketcher
? Set to the standard orientation (with shading on)
? In the Dashboard set the following if necessary:
o Revolve as solid
o Set to revolve through 360 degrees
? Complete the feature
If you are having trouble existing sketcher or creating the revolve section then the chances are the sketched objects do not form a closed loop e.g. a line is missing, two lines not quite meeting or maybe intersecting lines overlapping. So check that all the lines are there, in particular the base line. Then you can check for gaps and overlaps. The commands in the Sketch> Inspect panel as shown in figure 3.39 should assist in identifying these sketching errors. If the problem still persists check that you created the axis of rotation using the correct centerline type.
Figure 3.39: Sketcher diagnostics
To finish the part
? Create a straight ?25 hole that is coaxial with the Roller centre axis
? Now add the 6 mm rounds
See figure 3.40.
Sketch inspection / diagnostic tools
Module 3 – Exercise 2 – parts and assembly 3.29
Figure 3.40: Roller creation
Save the part.
Module 3 – Exercise 2 – parts and assembly 3.30
3.6 Part development: spindle and bush
3.6.1 Creating the spindle
Create a new part called Spindle.prt. We are going to create a two sided solid extrusion with an internal sketch. Display the standard orientation and datum planes.
Figure 3.41: Spindle
? Choose Extrude
? Select the RIGHT datum plane
? Sketch a circle that is centred on the origin, and modify its size to 20
? OK sketcher,
? From the Dashboard set the depth option as Extrude on both sides of the sketch plane… and change the depth to 100
? Complete the feature
We are now going to remove material from each end to create the machined shoulders.
? Select Revolve tool
? Select the FRONT datum plane as the sketching plane
? Set the sketch view
As you go through the following instructions also refer to figure 3.42.
? Open the References window (Setup panel)
o Pick the top surface of the cylinder and the right end of the cylinder as sketch references. You should now have four REFERENCE to choose from
o Close
? Insert a Geometry Centreline (Datum panel) through the centre of the cylinder – this will be the axis of revolution
Module 3 – Exercise 2 – parts and assembly 3.31
? Insert a vertical Construction Centreline (Sketching panel) mid-way through the part i.e. coincident with the RIGHT datum plane
? Sketch two lines to represent one of the machined shoulders. Change the diameter to 12 and the shoulder to shoulder distance of 66 as you did for the shoulders on the Base part.
? OK to exit sketcher.
Figure 3.42: Spindle first shoulder
Set to standard orientation with shading on.
From the Dashboard
? Revolve as solid
? Remove material (make sure that the directional arrow is pointing away from the part)
? Complete the feature
Mirror the shoulder feature about the RIGHT datum plane to create the second shoulder.
Add a 2x45O edge Chamfer to each end of the Spindle as shown in figure 3.43.
Figure 3.43: Spindle second shoulder and chamfers
Geometry Centreline
Construction Centreline
Additional references
Module 3 – Exercise 2 – parts and assembly 3.32
Create a straight hole (5.1mm diameter) starting on the end face of the Spindle and coaxial with the centre of the Spindle.
From the Dashboard
? Set to the Standard hole profile and Drilled hole to shoulder depth as highlighted in figure 3.44
Figure 3.44: Straight hole
? Drill to a specified depth of 50 mm
? Complete the feature
Before creating the radial grease hole we need to insert a reference axis. This will be along the FRONT and RIGHT plane intersection.
? Turn on the axis display
? Create a Datum axis (Datum panel)
? Select the FRONT plane (if your plane display is switched off you can select the FRONT plane from the model tree)
? Hold down the key and also select the RIGHT plane
? OK the Datum axis window
? Hole tool
? Select the outer surface of the cylinder and the radial axis (remember to hold down the Ctrl key)
From the Dashboard
Module 3 – Exercise 2 – parts and assembly 3.33
? Set to the Standard hole profile and Drilled hole to shoulder depth as highlighted in figure 3.44
? Drill to a specified depth of 14mm
? Complete the feature
Save the part.
Figure 3.45: Completed spindle
Change the display to Hidden Wireframe and set the view orientation to Front. Note the appearance of the bottom of the holes. Change the display back to shading.
3.6.2 Creating the bush
Here is one for you to attempt by yourself – create a new part called Bush.prt that is a revolved solid.
Figure 3.46: Bush
Module 3 – Exercise 2 – parts and assembly 3.34
3.7 Assembly of parts
3.7.1 Before you start
Go back to each part and apply an appearance change so that the parts are different colours. Refer to section 2.21 for revision if necessary. Avoid Creo selection and highlight colours. Save each part again.
Think carefully about how you would actually assemble these components. Your modeling process should reflect this. I would first place the Base on the workbench. Then place one Bracket approximately in the correct position (mating the two surfaces together), push the Bracket up against the shoulder (making the faces coincident), and line up the holes or the outside edges. Then I would press the two Bushes into the Roller to make a Roller sub-assembly. Press one end of the Spindle into the Bracket, slide the Roller sub-assembly onto the Spindle, then slide the other Bracket into position. Of course, in a real assembly we are also including bolts or screws. You can add these later if you wish.
3.7.2 A simple assembly
We are going to create a subassembly consisting of the Roller and two Bushes. This models the process that we would follow when assembling the real device.
If necessary set the working directory to the Roller_Bracket folder where all the parts are filed. Create a new assembly file called MyRoller.asm. You may have to force the New File Options window to appear by first unchecking the Use Default Template box in the New window. Set the mmns units if necessary.
Figure 3.47: Creating an assembly file
You will note that default datum planes are also created in assemblies. However, if you cursor over them you will notice that they are now called ASM_FRONT, ASM_RIGHT and
Module 3 – Exercise 2 – parts and assembly 3.35
ASM_TOP. To display them in the model tree you will need to set the tree filter to include features – refer back to figure 2.27 in section 2.13 if you need to..
From the Component panel choose the Assemble icon and open the Roller.prt.
The Roller will either attach itself to the screen or it will float around with the cursor. If the latter, move the model to any position on the screen and then click to temporarily place it.
Next we will specify exactly where we would like this base component positioned by referencing it to the assembly datums.
Expand the constraint type box in the Dashboard – see figure 3.48. Spend time previewing the options that the list contains. You assemble parts by applying constraints to entities such as edges, planes, surfaces, etc. Each constraint has a unique application. Automatic leaves the constraint decision up to Creo and this, in turn, is based on the model elements selected by you.
At present, the Roller is sitting at an unreferenced position in space and its placement status is no constraints as shown in the Dashboard. A part must be fully constrained to be part of an effective assembly. It is possible to add or delete constrains as sometimes Creo or we get it wrong on the first attempt.
The bottom icon in the constraint’s list is used to assemble component at the Default location. Choose this now and the Roller should be placed so its datum planes are coincident with the assembly datum planes. The Roller should now be fully constrained. For this course we will always use the Default constraint for locating the first part in an assembly.
Figure 3.48: Constraints box
or click to complete this placement. Switch off display of datum planes.
Module 3 – Exercise 2 – parts and assembly 3.36
Select the Assembly icon and open Bush.prt. Drop it on the screen away from the Roller model if you are given this option.
If the Bush is placed such that it is hidden or partially hidden by the Roller you will need to move it in order to expose an element for selection..
To ‘move’ or ‘translate’ just the Bush:
? depress both and keys while holding down and then move the mouse
You can also roll or rotate the incoming model:
? depress both and keys while holding down and then move the mouse
A more interactive method of moving the bush is by using the 3D Dragger. This option can be toggled off and on with the icon in the Dashboard. When this is activated the model is displayed with movement indicators as shown in figure 3.49.
Figure 3.49: 3D dragger
You now have the ability of dynamically moving and rotating the model in every direction through selection of the dragger elements:
? arrows
? translucent quadrants between the arrows
? small sphere at the centre of the arrows
? coloured circular arcs
You should experiment now using this technique. There is also a short video on ‘Orienting Components’ on the homepage of the Learning Connector (top right corner of the screen).
Once the Bush is clear of the Roller click on the outside surface of the Bush. At this stage Creo is adopting an automatic constraint which can be confirmed in the Dashboard and also in the flyout annotation box – refer to the first diagram in figure 3.49. Now select the
Module 3 – Exercise 2 – parts and assembly 3.37
hole in the Roller. This should have created a coincident constraint and the Bush will have moved to obey this constraint – figure 3.50, second diagram.
Figure 3.50: Assembling the bush
Note that the Bush is only partially constrained, refer to the status in the dashboard. Creo will be waiting for you to nominate another constraint. Select the little shoulder on the Bush –figure 3.51. Before choosing the next surface change the constraint type (now probably automatic) to coincident either in the Dashboard or in the constraint annotation pop-up menu which can be displayed by button down when the cursor is on the Automatic annotation – see figure 3.51. This demonstrates how we can force or override a constraint. We could have left it as automatic and hoped that Creo would get it right.
Figure 3.51: Assembling the bush
Now click on the mating surface of the Roller –figure 3.52.
Module 3 – Exercise 2 – parts and assembly 3.38
Figure 3.52: Assembling the bush
The Bush is obviously facing the wrong way as shown in the first diagram of figure 3.53. Click on the Change orientation of constraint icon in the dashboard to turn the Bush around. Refer to figures 3.53
Figure 3.53: Assembling the bush
Creo shows this assembly as fully constrained as it assumes that the angular orientation of the Bush in the hole is not critical which it isn’t. So we can accept this and complete the placement by or clicking.
Now assemble the second Bush. First rotate the Roller so you can clearly see where the bush needs to be placed.
Save the subassembly.
Create a new assembly called RollerBracket.asm. This is the main assembly. Set units.
Module 3 – Exercise 2 – parts and assembly 3.39
Add a component (Base.prt) and constrain it by using the default location placement option.
Add a component (Bracket.prt). Creo will probably assign the correct constraints as you select the surfaces but if it doesn’t then you can force the appropriate constraint as mention previously. All constraints should be coincident. Choose the surfaces as follows while also referring to figure 3.54:
? The ‘underneath face’ of the Bracket and one ‘machined upper face’ of the Base.
? The ‘leading face’ of the Bracket foot and the ‘machined shoulder lip’ of the Base. (You may have to force the coincident constraint here.)
? One Bracket hole and the corresponding Base hole. (It is more important to constrain the holes rather than the outer cast edges)
? ? or click to complete the placement
Figure 3.54: Assembling the bracket
For modeling purposes it does not normally matter in what order the constraints are selected but it is good practice to choose an order that reflects how the real parts would be put together.
Add a component (Spindle.prt) by inserting the Spindle into the Bracket hole and mating (coincident) the two edge surfaces together. Creo will show this as fully constrained and you could accept this. However, if we needed to orient the spindle’s radial hole at some particular angle we could do so. First we need to create a new constraint in the Placement tab – refer to figure 3.55.
Module 3 – Exercise 2 – parts and assembly 3.40
Figure 3.55: Adding a new constraint
Turn on the datum axis display. You may want to turn off the 3D Dragger for a clearer view. Now pick the axis of the Spindle’s radial hole and then the surface of one of the Bracket machined faces – figure 3.56. Change the constraint to angle offset. When you do this you will be given the option to edit the angular dimension. Try it and see if you can orient the hole so that it is 45o to the Base and pointing towards the front of the assembly.
Figure 3.56: Assembling the bracket
or click to complete the placement.
Add a component (MyRoller.asm). Insert the Spindle into one of the Bush holes for the initial placement. For the second constraint choose the end face of a Bush head and the inner
4 edit this value
New constraint
1 select axis
2 select face
3 change constraint
Module 3 – Exercise 2 – parts and assembly 3.41
face of the Bracket boss. Chance the constraint type to Distance if Creo does not choose it for you. Set the offset distance to 1 mm (or -1 mm) to create the clearance gap between the two parts – see figures 3.57 and 3.58.
Figure 3.57: Assembling the bracket
or click to complete the placement.
Add a component (Bracket.prt) and place this component using the same procedure as the first Bracket.
Save the assembly.
Figure 3.58: Roller bracket assembly
clearance gap
Module 3 – Exercise 2 – parts and assembly 3.42
3.8 Doing things smarter
We could have saved the sketch we used in developing the Bracket, and used this sketch in the Base. We could also create new parts in the assembly mode and build these parts from the existing ones in the assembly. With a little thought, I am sure you can think of more helpful modelling strategies.
3.9 Relations
3.9.1 Part relations
In the future there may be a requirement to make larger Bases with larger hole spacings. Our current dimensioning scheme allows for this. However, larger Roller brackets may also require larger bolts – in which case the current round size of R12 on the Bracket and Base may be too small. Rather than expect the designer to remember to change all of the dimensions, we can include relations to force some dimensions to be based on others. The independent dimensions are sometimes called Driver dimensions and the dependent ones are sometimes called Driven dimensions.
Open the Bracket.prt.
To add a relation you will need to open up the Tools tab.
? In the Model intent panel choose Relations
A Relations window will open. In this window:
? Check that Part is set in the Look in box
Select the ‘foot’ feature of the Bracket
You will notice that the dimensions are now displayed in code as symbolic dimensions. Place the cursor over the R12 round dimension. On my model it is shown as Rd11 [d11:F5 (sketch_1)] see figure 3.59. This means that the round dimension is the 11th dimension entered for feature number 5. Feature 5 being the foot of the Bracket. Your name will most likely be different.
Module 3 – Exercise 2 – parts and assembly 3.43
Figure 3.59: Selecting symbolic dimensions for a parametric equation
? Click on the dimension name for the round. The name should now appear in the Relations window
? Key in ‘=’ or press the equals icon on the left side of the Relations window
? Select the 12 mm hole to display its dimension name then click on it. The relation equation should be displayed in the Relations window – see figure 3.60. (The relation required is ‘round radius equals hole diameter’. In my part this relation is d11=d40)
? You can add more relations at this time, or hit OK to accept relations
The round size is now dependent on the hole size – i.e. if the hole size is changed then the round size will be updated automatically.
Module 3 – Exercise 2 – parts and assembly 3.44
3.60 Relations equation
To test the relation
? Repaint screen
? Select the hole and Edit the 12 mm dimension. Make is 20 mm
? Regenerate the model
The model should change to reflect the new sizes.
Now try to edit the round radius – you will not be able to because this is a driven dimension – read the message below the graphics screen.
Change the hole diameter back to its correct size and regenerate. You can use part relations to force many of the dimensions to be driven from a small number of key ones. Spend sometime trying this now.
To edit relations
? Tools >Model intent panel then choose Relations
? Set Part in the Look in window
? Edit the relation equation when it is displayed in the window. Try incorporating a constant.
? When done – highlight the equation then Delete it
? OK to accept changes
Make sure that you change all the sizes back to their original values and then Save the model.
Module 3 – Exercise 2 – parts and assembly 3.45
3.9.2 Assembly relations
Open the RollerBracket assembly. We are going to set up a relation such that the round on the Base will be the same as the round on the Bracket foot.
To add an assembly relation you will need to open up the Tools tab.
? In the Model intent panel choose Relations
? Check that Assembly is set in the Look in box
? Select the Base part to display the dimension names
You will note that the assembly relation dimensions are written slightly different to the part relation dimensions. This is because the dimension name now includes the part number, for example Rd2.4 means dimension 2 on part 4.
? click on the dimension name for the round. The name should appear in the Relations window
? Key in ‘=’ or press the equals button on the left side of the Relations window
? Select the ‘foot’ of the Bracket to display its dimensions
? click on the dimension name for the round
? OK
To test the relations
? Refresh screen
? Open the Bracket.prt
? Select the ‘foot’ feature and Edit the round size to say 20 mm
? Regenerate the model
? Activate the RollerBracket assembly
? Regenerate the model
The model should reshape.
Now attempt to modify the radius of the Base – it should not be possible as it is the driven dimension.
Change the Base round back to 12; Regenerate both models and then Save the assembly.
Incorrectly applied relations can cause very strange errors in your parts – be careful and plan before you start changing things. The order in which relations are applied is very important. Spend some time now adding assembly relations. Delete them when you are finished playing around.
Module 3 – Exercise 2 – parts and assembly 3.46
3.10 Cutting / sectioning an assembly model
3.10.1 Creating a section cut
Assembly models can be cut or sectioned to reveal internal parts by removing specified sections of the model.
? open the RollerBracket.asm
? Decide what section to remove. For the Roller bracket we will remove one quarter of the model. This is ideal for models that have parts or features arranged symmetrically about two perpendicular planes.
? Select the FRONT ASM plane
? Sketch
? Set the sketch view
? Create a rectangle to encompass the right half of the model as shown in figure 3.61
? exit Sketcher
Figure 3.61 Cut sketch
? Standard orientation
? Extrude
? Make sure that the extrusion is directed towards you
? From the Dashboard
o Choose Extrude to intersect with all surfaces as the extrusion depth
o Click on the Intersection tab and deselect Automatic Update from the Intersect window – see figure 3.62. You can now remove the parts that you don’t want cut e.g. the Base and the Spindle. In the window mouse over BASE then click and select Remove. Also remove the SPINDLE from this list.
Module 3 – Exercise 2 – parts and assembly 3.47
Figure 3.62 selecting parts not to be cut
o Close the Intersect window by clicking on the Intersection tab
o Complete the feature
Figure 3.63: Assembly model showing a section cut
You should now Suppress this feature (refer to section 2.13) so the model is complete. You can always bring the ‘cut’back with the Resume command.
Save the assembly.
Untick Automatic Update
Module 3 – Exercise 2 – parts and assembly 3.48
3.10.2 Dynamic sectioning
With the Roller Bracket assembly open select the View tab and then from the Model Display panel choose Section Z Direction – see figure 3.64.
Figure 3.64: Dynamic section setup
Grab the directional arrow in the model to dynamically move the section plane through the assembly. – see figure 3.64.
Figure 3.64: Dynamic section
Module 3 – Exercise 2 – parts and assembly 3.49
Parts can be excluded from the cut by selecting them in the Dashboard’s Models tab – see figure 3.65. The cut surfaces can also be highlighted by using the colour tool in the Dashboard.
Figure 3.65: Excluding parts from the section cut
Complete the feature and then Deactivate (from button pop-up menu) the XSEC…… feature in the model tree. If this is not displayed in the model tree then you will need to set the filter to show Sections – see figure 3.66.
Figure 3.66: Displaying sections in the model tree
Save the assembly.
Module 3 – Exercise 2 – parts and assembly 3.50
3.11 Hiding a part or feature
Another convenient way to inspect internal or hidden parts of an assembly is to hide exterior parts. Expand MYROLLER.ASM from the model tree and select the ROLLER.PRT. click to show the pop up menu then select Hide. The Roller should disappear from the assembly model and its name will be greyed out in the model tree. To display the Roller click on the model tree ROLLER.PRT, click to show the pop up menu then select Unhide.
It is also possible to hide certain features of parts e.g. cosmetic threads can be hidden to improve the assembly model display in any of the wireframe modes.
3.12 Saving an assembled model
As mentioned previously, in Creo a new file is created each time you save. One method to prevent your directory getting too cluttered and once you are happy with the final versions you can remove the previously saved versions by
? From File>Manage file>Delete old versions
? Accept
This can be a tedious method especially if you have many assemblies, including sub assemblies and parts, as you need to do it for each model.
Another technique keeps the ‘last saved’ version of the assembly model and the ‘last saved’ versions of all the model files associated with that assembly in one go. When you are satisfied that your models are correct create a new folder in your directory. This is best done using the computer’s file manager e.g. My computer or Windows Explorer. Your final versions will be copied to here. With your assembly model open …..
? From the top menu File>Save as choose Save a Backup
? Navigate to the newly created folder
? OK the Backup
All the model files associated with the assembly model will have now copied to the new folder.
The assembly model displayed on the screen will be that copied to the new folder.
This technique will only copy the model files. The drawing files will not come across. If you require the drawing files I suggest that you back them up individually or manually copy and paste them using the computer’s file manager.
3.13 Renaming your model
Finally, if you have reason to rename your model do it under File>Manage File>Rename. Do not rename the model files using the computer’s file manager. This is very important when dealing with assemblies consisting of many parts.

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