Ashebots #7300 PTC Creo Parametric Assembly Tutorial
I assume there are a lot of mentors (like me) who would like to use Creo but have little-to-zero mechanical engineering training and find it too overwhelming to even get started. So I wrote this with that audience in mind. I've had considerable experience with 3D software (such as Blender) which helps a lot.
You need a pretty solid computer to run Creo - they’ve probably got minimum-system requirements online somewhere.
You have to have a 3-button mouse to use Creo (and pretty much any 3D software). If you’ve got a scroll wheel, it probably ‘clicks’ as well and you can use that.
Initial Screen
If you haven’t already, go into your Favorites folder here and add shortcuts to the folders containing the Tetrix models, test projects, etc. you use.
You won’t make any Parts for a while - you’ll use the supplied Tetrix Parts while creating Assemblies.
Assemblies
A Part is a single physical thing: nut, bolt, washer, gear, c-channel, etc. The files have a .PRT extension.
An assembly is a collection of those parts: i.e. a robot. These files have a .ASM extension.
Inside those assemblies, those parts aren’t just positioned to look like what you want to create. They are linked via how they should react as physical matter in relation to the other parts. This is what enables you to eventually create joints and gear mechanisms and drive them with motors/forces.
Even more fun, assemblies can include other assemblies!
EVERY TIME you open Creo, set the Working Directory. Here’s a good reason to have that Favorites folder ready! Set it to where you segregate your assemblies or the central Tetrix Parts folder if you keep them together. File - Manage Session - Set Working Directory.
Create an Assembly
So, select File - New. Change the Type to Assembly and have a good Name ready! It’s difficult to rename these later, so know what you’re doing ahead of time. i.e. not like this one. OK.
Main Assembly Screen
Don’t let all these buttons scare you - yet.
Some of the key areas are noted here. It’s easy to get lost. It will be a while before you get off of the Model. tab, so make sure you have it selected if things get too weird. Think of it as your home screen.
- Regenerate the underlying whatever behind this assembly. Does error checking and such. You can’t save an assembly if it’s got errors in it.
- Assemble allows you to grab a new piece for your assembly.
- Model Tree displays the hierarchy of the Parts and Assemblies that comprise your Assembly.
- Named Views jumps to TOP, LEFT, etc.
- Datum Display Filters are things you’ll soon be futzing with, but for now turn them off if you like.
Click Assemble and navigate to FTC_Tetrix_KOP_Block_Party\Tetrix_Kit_FTC. (which might or might not be your working directory)
The Open dialog opens and there’s a Preview button in the lower right corner. Click that and you should see something like this:
Find our friend tetrix_739068_2012.prt and Open. and you’re placed in Component Placement.
Component Placement
Note you’re not in the Model tab - this window is more like a dialog with the green check and red X acting as OK and Cancel. But a middle-mouse-button click is the same as OK so it’s easy to accidentally close this screen because you were really trying to do a middle-mouse-button drag to rotate and not even notice.
This is a vital screen, so let’s see how to get back into it. Just click the green check to get back to the Model tab. You’ll see the part added as a child to your MYASSEM.ASM. We want to get back into its Component Placement tab - so select the tetrix entry in the Model Tree, right-click to get the context menu and select Edit Definition.
This takes us back to Component Placement so we can set the component’s constraints.
There has to be one piece of the assembly that acts as the ‘ground’ for all the other parts. We’ll use this part by selecting Default from the constraint drop down. Note that our part has turned gold - that means it’s the base. Green Check it.
Let’s attach another Tetrix part to this. Click Assemble and find 739061:
And we’re back in Component Placement with our new piece.
Only a single component can be placed here. Right now, we’re attaching this little strip to the c-channel.
Once things start getting complicated, you’ll find yourself jumping in and out of Component Placement to get all the pieces to connect properly.
Let’s attach it so it’s flush against the side of the c-channel, pointing upwards.
This screen is somewhat bewildering - but probably has to be.
Take note of the Placement dialog/tab. You’ll probably have to click it to open it. When a component is fit into your assembly, it’s done through (usually) numerous constraints. You can go in here to fixup the inevitable mistakes along the way.
Coincident is your go-to constraint and I’ve selected it here. The two right arrows point to things to help de-clutter your screen.
Creating these constraints is a multi-select process. Creo is good about stepping you through it, but you’ll need to be able to navigate. In the Placement window, our Coincident constraint is listed. Right now, neither Select component item or Select assembly item is highlighted. These tell Creo how to use the piece we’re about to select. Highlight Select component item and select the top face of the new piece.
Note that Creo has selected the Select assembly item constraint prompt and your mouse pointer now has a line back to the component item: Creo is asking you which assembly item completes the constraint. Click on the right, vertical face of the c-channel and WHAM - connected.
The circle-with-arrows at the top is the tool that allows you to position the new component. This tool also obeys the constraints you’ve defined. If you turned it off, turn it back on.
Note that certain movements and rotations are disabled.You can slide the flat piece along the side of the channel - you can even slide it up, down, left or right off of the entire channel. That’s because all we’ve really constrained so far is that these two surfaces stay on the same plane.
In the Placement window, click new constraint that appears beneath our Coincident constraint. A new constraint will be started - of type Automatic - and you’re prompted for the assembly item. We want to constrain the large hole at the bottom of our component to one of the similar holes on the channel. Start out by selecting the interior of the component’s hole. Creo will highlight each half - it doesn’t matter which you pick. Basically, you’re selecting the cylinder that runs through that hole and off into infinity in either direction. Whoa.
You’re being prompted for a similar construct on the assembly so click the interior surface of the next larger hole up that has four smaller, surrounding holes and - shazam:
Notice that our new component is now gold. It is Fully Constrained. It can’t be moved. Notice also that our Automatic constraint is now Coincident.
Now, if you stop and think about it, the little strip should still pivot/spin on the holes we connected. But Creo is telling us it won’t do that. That’s because Allow Assumptions is checked at the lower right of the Placement window.
Turn off Allow Assumptions and turn on the manipulator tool if it isn’t already and visible. You’ll see you can now rotate the strip as you might expect. That’s handy most of the time - but it can lead to confusion if Creo is making assumptions you don’t want.
Re-enable Allow Assumptions and Green Check the changes.
Save your assembly so you can experiment and practice. As an exercise, add another strip to the channel but disable Creo’s assumptions and mount it so it’s at 45 degrees to the channel.
Navigation/Manipulation
You need a 3-button mouse. Your scroll button usually works; if not, go into the mouse settings and make sure clicking the scroll button is a ‘middle click’
Ctrl+d is the most important keyboard shortcut when learning to move around in 3D space - it returns you to the default view. It’s easy to get disoriented or scroll off into outer space. Ctrl+d.
Mouse 3D Movement
Roll Scroll Button | Zoom In & Out. | The zoom happens around the mouse cursor - helpful for zooming in on particular areas. |
Middle-Click, hold & drag | Rotate | Show/Hide the Spin Center to control rotation center: mouse position or its center-of-gravity. |
Mechanics
Gears
Create a New Assembly, add a long c-channel (739069) with the Default constraint.
Add a small gear (739028) and use a Pin constraint to attach it to the base:
Back in the Model tab, active Drag Components, click once on the gear and you should see it move as you move the mouse. If not - go back and review your Pin constraint.
Close the drag tool and add a big gear (739086) and Pin constrain it to the base so it lines up with the small gear.
Invoke the Drag Components tool again and verify both gears turn.
You might have expected them to turn each other - but they didn’t. For that to happen, we have to define the mechanics in Creo - because it has no idea those two things are gears. They just happen to look like gears to you.
Mechanics Application
Go the the Applications tab and click the Mechanism button.
Note there’s now a Mechanism Tree under the Model Tree and a new ribbon.
Define a new gear connection by clicking Gears in the Connections ribbon group. (or expand the Connections node in the Mechanism Tree, right-click Gears and select New) Either way, the Gear Pair Definition window is opened.
The highlighted arrow button under Motion Axis is telling you to pick the axis of rotation for Gear 1. The available choices are shown as the orange lines/arrows in the center of the gears. Click on the axis in the small gear and enter 1 in Pitch Circle’s Diameter field.
Select the Gear 2 tab, pick the large gear as the Motion Axis and give it a Diameter of 4. and click OK.
Your new mechanism is available in the Mechanism Tree and represented by the small green gear glyphs.
Right click on the tree node for a context menu and Edit Definition to re-open the Gear Pair Definition window to adjust gear parameters.
Now activate the Drag Components tool (available in the Mechanisms ribbon as well) and see that turning either gear causes the other to rotate.
Note especially that the gear diameter ratio is used:
- turning the small gear spins the larger gear slowly - torque
- turning the large gear spins the small gear quickly - speed
Motors
These gears aren’t going to turn themselves and we’re not going to stick our fingers in there and do it, so let’s add a motor.
If not already there, go back to Mechanisms under the Applications tab.
Add a force motor via the ribbon button Insert or context menu the Mechanism Tree. This opens the Force Motor Definition window.
Select the axis to be driven by this motor: click on the little orange glyph in the gear (not the green gear glyph). Pick the same axis the small gear uses.
Under Magnitude, enter 100 for A.
Click OK. The inset show the new force motor (the green twist glyph) on that axis.
Mechanism Analysis
Note: at this point, my knowledge level drops to almost zero. It seems like there should be an easier way to get this motor running - but this is all I know…
Click on the Mechanism Analysis button in the ribbon (or tree) to open the Analysis Definition window. The Preferences tab specifies the length of time we’re going to run the mechanism.
Leave all that alone and go to the Motors tab to make sense of the choices in the Type drop-down list.
Note that no motors are listed for the Position or Kinematic types. The force motor we just created is listed under the other 3 options. Select Static then Run.
You should see the small gear driving the large gear for a while - then stop. OK this window and the new analysis appears in the mechanism tree. Right click and Edit Definition to tweak the parameters and re-run the analysis.
Troubleshooting
File, Manage Session, Select Working Directory
Navigate to the directory containing the parts and set it as your working directory. Regenerate the assembly and the PRT files will be set properly.