Parameters in Drawings?
Yeah, I know they're working on it. Presently you can't even create custom text parameters in the model to pass into a drawing because there's some sort of a limitation on how they are stored in the cloud. But it's being addressed. But the inability to access model parameters from drawings is a major flaw.
I can expand a little on how dimensioning works in Creo drawings if anyones interested. I found that most people outside Creo never heard of this approach but I find it vastly superior to how everyone else (including Fusion) does it.
Take simple part like this -
It is defined by 4 dimensions, there they are all in the sketch already -
If I were to do a drawing in Fusion I would have to position a view and then put those dimensions in by hand or use autodimensioning that would offer me a range of dimensioning options.
But why do I have to dimension it if I already did? In Creo you position a view, then right click the rotate feature (they got feature tree available in drawings) and select "Put dimensions on select views", then select the views. Dimensions appear on those views. You can then double click them in the drawing, change the value, regenerate and the drawing will regenerate the model. Dimensions are parameters. Not random measurements taken from 2D objects.
This achieves several things:
1. You never leave any model feature undimensioned in a drawing and never forget anything. Nor will you ever overconstrain a drawing by mistake. All you have to do is just go feature by feature from the bottom of the feature tree to the top. Works like a check-list. Very useful for large drawings with multiple sheets and dozens of views.
2. Your drawing is the exact detailed annotation on how the model works. Ofcourse there's also an option to put in any reference dimension by hand just like you do in Fusion. There's nothing stopping you from having a sketch like this where all the dimensions are wrong (nobody dimensions a machined part like this):
and then put correct dimensions in by hand in the drawing. But you quickly learn to not do it like that. And if you find that your dimension is off the wrong datum, rather than manually placing a reference dimension in the drawing you go back to the model sketch and replace it there. It may be a bit of a pain for a complex part, yes. But doing it right saves you time and effort when you need to make changes. And also makes the whole package easier to understand for others and for your future self. It creates beautiful models with neat feature trees because you suddenly don't want to randomly extrude things on top of each other or cut things randomly anymore. You want to do it right, have the dimension off of the correct datum and have no more features than you have to. Because you'll thank yourself later on when it's time to do the drawing - half the work will be already done.
3. Dimensions never disassociate (something that plagues Fusions drawings all the time). Because dimensions are parameters, not just random measurements from point to point. Accessing a dimension from the drawing is the same as accessing that parameter from a model sketch, or from Parameters table. They are the same thing.
They also contain tolerance information. You can use these parameters. You can reference them in technical text, tables, anywhere.
@flatout3d, in the snapshot of your configured part, it shows that you set "=Post_Length" to the "Landscape Tie" which is an internal component. But in the snapshot of the drawing, you want to display the descriptions for configurations Post ID 1, 2, 3. To do this, please right-click the root component "Config Part BOM Test v1", then enter the description in its Properties dialog. This setting can also be done in the Configuration table, Properties tab (attached snapshot). Then the description will be shown in the drawing's parts list.
Evan Gu
Inventor/Fusion QA Engineer
