Split body - how to keep surfaces in new created part from body

[Szymon.Biela]

Good morning everyone,

I found that split body option is very atractive for a way of designing for my company and i would like to introduce it for other designers. Before i do that, i need to solve one problem and thats why im asking you for help.

Problem:

I have part with M10 holes in pattern and i want to divide this part in two separately with SPLIT BODY option. After dividing a part i use CREATE PART FROM BODY to save new part. 

Everything is ok until i open new part. new part is missing surfaces (for example - threads of M10 holes).

I cannot find any solution for this problem.

If anyone has idea how to copy it or at least, how to mark thread after split body divinding, i will be very grateful.

FYI, i work in CREO 7.

best regards,

Szymon Biela

[tbraxton]

Bodies are solid geometry. Surfaces are not part of a body in Creo so you should not expect any surface geometry to be included with body operations. If you need to copy surfaces from one model to another in a top-down fashion you will need to use other functionality (i.e. copy geometry).

For your threaded hole locations, you can control this in other ways and share the locations between models. If you explain the design intent you want to manage in more detail, someone will offer some suggestions.

[Szymon.Biela]

We are designing progression tools and let's take top plate as an example.

Sometimes during project we work on, we decide to divide top plate into two smaller. this plate already has holes etc.

i would like to use split body tool, because it works really good for (as you mentioned) for solid geometry. unfortunatelly, in new created part from body i will lost not only thread surfaces (i think that it is worst for us right now) but also axes, points etc. it will be naked solid geometry. 

in this case, i will have huge difficulties at 2D drawing step because right now for threaded holes, we tag them on external diameter that is a surface in model. tag is diameter + M in front of it.

i am open for any suggestions.

[Pettersson]

 "Save as part" just creates a part with a Copy Geom feature, so you can edit that feature to bring along additional geometry. Edit the definition of the Copy Geom feature in your split-off part. Go to "Surface Sets". In the selection filter (bottom right in your Creo window), select "Quilt". Now select each threaded hole. That should get you to bring the thread surfaces along with the body.

[tbraxton]

This will work (adding elements to the copy geom) but if you expect to have access to the dimensions used to locate the holes in the master model as an example, they will not be available in the derivative part. If you create 2D drawings or used MBD then you should consider the work required to be able to display the desired annotations, datums, etc.

Consider how to best leverage the derivative models based on your workflow and deliverables.

[Pettersson]

OP wrote "we tag them on external diameter that is a surface in model. tag is diameter + M in front of it", which I interpret as adding driven dimensions in the drawing, but I may be wrong. If you want to keep the annotation history, "Save as part" is not the way to go, unfortunately, but this is not important to everyone. Lot's of companies make drawings largely using driven dimensions in the drawings.

The Copy Geometry feature supposedly has a tool to copy annotations, but I don't think I've ever managed to get that to work.

[Pettersson]

By the way, since you wrote you have a hole pattern: You can also make a new Copy Geometry feature and add the thread surface of only one of the holes. Then you can make a reference pattern of that Copy Geom feature. This can be handy since it allows you to use that for other features or when assembling screws, for example. Another downside of the "Save as part" function is that you lose the pattern information and thus the possibility of doing ref patterns. But with this trick you can still do ref patterns (but only when selecting the thread surface as a reference, not if you're assembling a screw to the solid cylindrical hole surface, for example).

[Szymon.Biela]

Thanks for replay. i know this is possible but this solution is only good if you have to do it one time.

For big plates with hundred of threads, multiplay parts, it will be horrible to click on each thread. waste of time in my case.

[Pettersson]

You can speed it up in several ways.

• You can drag the cursor to make a selection box.
• You can make a 3D selection box.
• You can use the search tool (search for quilts, search by feature of type hole).
  • You can automate this using a mapkey
  • This will find all thread surfaces, though, no matter on what body. Don't think there is a way to search for features depending on the body, and if the holes are made before the split, that probably wouldn't work, anyway.

You can also make a new part, use Merge/Inheritance to get the entire old part. then use a Remove Body command to remove the bodies you don't want. That will get you the thread surfaces as well. Through it may have the opposite problem, with the thread surfaces staying behind after the body has been removed.

In general, threaded holes don't work great with multibody, as they are both solid geometry and quilts. Would be nice if these surfaces could be somehow "attached" to the body, but that's not how it works today, so you're left with these kinds of makeshift solutions, I'm afraid.

[vnamboodheri]

Hello @Szymon.Biela, 

It looks like you have some responses from some community members. If any of these replies helped you solve your question please mark the appropriate reply as the Accepted Solution. 

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Community Moderation Team.