Assembly cuts modeling, is there a better way?

[SH_10126272]

I am working with Creo 8 and mainly do modeling of assemblies.

My current workflow consists of me making a blank part. Normally a basic cube. Then importing that into an existing assembly and making assembly cuts to get the geometry references. I then use those in the modeling  environment as relations to drive my sketches and modeling.

I find that this workflow is very clunky and requires me to go back and forth repeatedly to get it right. 

Is there a better way of doing this where I can import only the geometry/references I want as sketches then model off of that?

Any help would be much appreciated.

[tbraxton]

In general, you should avoid making assembly cuts. You have many top-down design tools that will support the design intent you need. Are you familiar with skeletons, copy geometry features, or multibody modeling?

[SH_10126272]

Thank you for the reply. I've only been using Creo for about a year so pardon my ignorance.

Im not familiar with skeletons.  Could you please explain and point me in the direction to learn more?

As for copy geometry and multibody, I took the class on them but I haven't really used them in the assembly environment to make geometry at the part level. 

[tbraxton]

Here is an introduction to skeleton models used for top down design.

Intro to Top Down Design Skeleton Models | Tutorial | PTC Learning Connector

I have worked on aircraft propulsion and structure design teams using Creo and the Top-Down Design methodology is typically used. For your specific scenario a skeleton would be created in a design to provide to you a space claim where your brackets must fit. This would also include any mounting points and mass property constraints.

You would copy this skeleton into all of the parts you are designing that are within the space claim and use it to create references to your designs. For an assembly of brackets mutibody modeling would be a strong contender rather than designing in assembly mode. In theory you can create a single part with all of the bodies that are required to design your bracket assembly. You would then create parts from body in your multibody master model and add them to an assembly representing the bracket components.

Based on your description you could create a single part using multibody and use a copy geometry to bring in the skeleton geometry. You can then design all components needed to build up the bracket assembly within this part.

[SH_10126272]

So I've been playing around with skeleton model and cant quite get it correct. 

I get to a point where I have either:

My sub assembly active with solid geometry that is tied to the skeleton, I see the outline of the feature but when I click away, it disappears.

Skeleton model active, solid geometry  tied to the skeleton, when I hide the skeleton it goes away (make sense that would happen) The problem here is how do I separate the solid geometry from the surfaces?

Or, a surface representation of the geometry that I cannot thicken.

It would be ok to design solid geometry that is tied to the skeleton but I cant save it as a separate body (so that I could export as a part to bring back into my assembly)

Any idea as to where I am going wrong? Hopefully this made sense. 

[tbraxton]

Without seeing your models, I may not be understanding the issue completely.

For skeleton models I would typically not have solid geometry in the skeleton. I define the intent using curves, surfaces, and datums. You would then use a copy geometry feature to add the skeleton features needed in the derivative parts of the skeleton.

Following this paradigm:

You should have a copy geometry from the skeleton in each of your bracket components that includes the needed references. With this approach you will be able to design in part mode only and in theory would not even need to open an assembly.

If you are working with multibody then mind the fact that bodies must include solid geometry. 

My suggestion to use multibody assumed that you would use a copy geometry from the skeleton in a single part model and then build the bodies needed to construct the bracket in this part. As you complete each body then you can create part from body to generate a part file for each bracket part.

Once you have the bracket parts then you would build an assembly representing the bracket assembly.

[BenLoosli]

What industry are you in?

What types of parts are you designing?

Many options that do not use assembly cuts to get what you need for reference into your designs.

[SH_10126272]

Im in the Aerospace sector working on bracket type parts.

My main hurdle is taking a number of parts, assembling them, and making custom mounting options for them to fit into a small area. 

[Patriot_1776]

Well....it depends.  You must figure out if the material IS actually removed at the assembly level.  for instance, when a couple parts are welded or bolted together and, say, a match-drilled hole is drilled at that level.  The key thing is that material removal actually DOES occur at that level.  If you're just using assy REFERENCES (almost always a bad idea) to get material removal that should be at the PART level, then you should be using skeleton or master model techniques.  You CAN actually just create curves and surfaces at the assy level to drive part geometry, and that is ok and truly top down and as long as you use those as reference and not OTHER PART geometry it doesn't create bad parent/child references.  I used to do that a lot, BUT, the caveat is that if you need to import geometry (like from vendor parts as STEP files), unless they changed things in Creo 8, you CANNOT import STEP files into the assembly.  So, THAT, is the only reason why I use skeletons.  I've burned myself a couple times like that, gotten into a design, and then found out I needed to import a STEP file, and then had to go ADD a skeleton part, and then put the surfaces and curves into that from the assy.  Tre annoying.  So, just to be safe, I always use skeletons now.

[mashton-2]

You could "save" while in the sketcher which saves the sketch to your working directory (or workspace in PDMLink) then import the sketch to your new part.

If the features are holes for mountings perhaps then you could drive them with a pattern table which you can save then import into new parts. Then you only need to create one hole using the hole tool import the hole table and adjust it  according to you needs.