Whats the most efficient way to use a "pre-processing part" multiple times in an assembly

[reignofratch]

So Say I have a default part size. For example, I can purchase plywood in 5x5ft sheets. I want all my dimensions of multiple parts to be based on that  full sized pattern. I might cut it into an L shape for one part, or into a foot wide strip in another. But they are all based on that one part.

Is it possible to import the fullsized sheet "plywood.prt" that already has material data attached, into an assembly multiple times to be placed and have extrudes cut from it using other constraints or will naming get in the way? Is there a better way to do this?

For other parts, like extruded aluminum with a complicated cross section, I'd only need to make the shape once, then cut it at different lengths inside the assembly, which would be phenomenal. Which is why I'd like to learn this now, while I'm only dealing with a project with simple cross sections.

[tbraxton]

You are describing an approach that would have assembly level cuts that are used to size parts to length (for the extrusion example). You should consider the ramifications of doing this in your environment, it may be good or may not be the best way to deal with this. Many Creo users would consider assembly cuts that only affect a single part within the assembly to not be a good practice. Think about it from the design intent standpoint before establishing this as part of your modeling workflow. This approach requires that  the assembly is in session to modify the length of a part (not optimal) and creates (arguably) unnecessary parent child relationships.

For your extrusion example I would control the length in the part and not establish external references to control the length. If your workflow requires that you modify the length in assembly mode you can do that by modifying the feature dimension within the part, not cut it using an assembly feature. If there is something in your workflow that requires the length to change based on use inputs or other design changes then you need to approach this from a top down strategy and establish design intent and control of the intent to determine how best to exploit Creo to manage your models. You should also take a look at the Creo Advanced framework Extension (AFX) if you are designing using extrusions or beams.

There are reasons to use an assembly cut but I would not use it for the applications you are describing if I understand your description accurately. You should explore some other tools which would likely better support what you are trying to do. Look at family tables, inheritance features, Pro/Notebook (layouts) skeleton models etc. to assess if they would be better options.

For your plywood example I would create a start part with the standard sheet and then modify it as required. Do you really need a model of sheet stock material? What value does a model of the purchased plywood add? I would just model the net shape part and assign the plywood material to the model.

Consider parts machined from purchased materials (sheet, rod stock etc.). I have never started from a model of the purchased stock of material to get a net shape part. For parts that are machined from custom forged blanks I would consider modeling the forged shape and using that as a start part to realize the net shape part. The reason being that the forging is critical to getting the net part to meet spec and I want to control it and it would be subject to inspection prior to post processing.

[rreifsnyder]

You could create a part with your base feature and use that as your template for creating the actual parts. You could then assemble the individual parts and in the assembly activate the part to create actual part features making the cuts you need. 

[reignofratch]

So how do you turn a part into a template?

[rreifsnyder · Accepted solution]

Assuming you are not using something like Windchill for data management, any .prt can be used as a template. Just save the part you are going to use in a convenient place like the working directory and then when you are creating a new part you can browse to that folder. There are ways to set the template folder specifically in the options also.

[reignofratch]

Nice! That's more than I'd hoped for. Thanks.