Boolean subtract

[scottm]

Assume I'm stupid... Not a stretch sometimes... I saw this discussed elsewhere, but the conversation got a little off topic.


I have a 30 feature part that I want to "subtract" from a block, i.e. design a mold. I have not used merge/quilt/ any of that much yet and will need a little detail as far as how to use it.


I come from a boolean background, so it was SO easy there, and I'm thinking its not here. Please correct me...


Thanks,


Scott

 

[lbotez]

In part mode use: Feature->Create->Data Sharing->ExtCutOut (Pro/E 2001).<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />


It allows you to subtract the solid geometry if an existing part from your current part. The parts are positioned one relative to the other by an overlapping 2 coordinate systems (one from the current one, another from the part to be subtracted). That's one way of doing a Boolean cut.


You can also copy surface geometry from one part to the other using External Copy Geom and then Cut Use Quilt.


Both methods can be used from within an assembly as well (CutOut and Copy Geom instead of ExtCutOut and ExtCopyGeom). In this case you need an assembly with both parts. The menu pick will be: Modify->Mod Part->Feature->Create->Data Sharing->.... The advantage of this method is that the parts can be positioned one relative to the other using all possible constraints (align, mate, insert...) rather then just a coord. system.

 

[scottm]

It looks like I'm burned again - I only have Foundation and do not seem to have most of the data sharing functionality. I did figure out how to do it in assembly mode - but at this point I'm just recreating the geometry from scratch (as cuts).


Thanks for the help

 

[jeff4136]

What version Pro/E? Is the volume you wish to subtract a closed quilt, solid, a collection of quilts and surfaces?

 

[scottm]

Its a solid. WF 2.0

 

[jeff4136]

Assemble the block(s) and toolbody. Activate a part you want to subtract a volume from. Insert, Shared Data, Cutout should get you started. There are other ways to go about it, but that's probably the most straight forward (?).
Edited by: jeff4136

 

[jeff4136]

... I did figure out how to do it in assembly mode - but at this point I'm just recreating the geometry from scratch (as cuts)...

Sorry, I need to learn to read. I'm not quite sure how you want to go about it?

 

[scottm]

If I had the data sharing (which Foundation doesn't have) I would use your method. I don't, so I'm not sure if there is even a way to do it in part mode.


It is implied in the docs that I could solidify a bastard (tool) shape and use that for a cut, but I haven't figured out how. I suspect I need to merge all the bounding surfaces on the tool into a "quilt" and then "solidify", but at this point it was just easier to go from scratch.


I appreciate your help - it seems like I could really use the data sharing module...

 

[jeff4136]

If I had the data sharing (which Foundation doesn't have) I would use your method.

 

[scottm]

I misunderstood you apparently, I was thinking you were saying how to do it in part mode. I did find the cutout in assembly mode. Its just that the resulting part is an assembly and loses some of its flexibility (i.e., you can't shell an assembly).

 

[jeff4136]

Ok, let's back up...

First, let me correct a bad choice of words that's confusing issues; change "have to have AAX to do it in assembly mode" to "do it within the context of an assembly".

So, again, if you have the block(s) and toolbody in an assembly: ACTIVATE the block part, then Insert, Shared Data, Cutout. This will essentially create (transparent to the user) an associative copy of the toolbody surfaces and perform the boolean subtract operation. It will be a "part feature" (vs. "assembly feature" which I'm assuming is what you've created?). You can then open the part and continue adding features as you will (may require setting a config variable?).

 

[scottm]

Ohhhhhhhhh..... Now I see what you are getting at. So that does accomplish exactly what I wanted, and its associative, and its a part.


Cool. I didn't even think to check to see if it had propogated back to the part level. My mind is not fully in PRO-E gear yet.


Perfect- thank you.


Scott

 

[jbuckl]

'cant shell an assembly' if you have 2 parts in the assembly, cut one from the other, (your boolean) and shell the 'other' part in part mode ie not in assembly.