Split a part into two pieces; two separate part files

[LeifMasrud]

I'm using wildfire 3.0 to create models of injection molding tools manually. (Don't want to shell out for Mold Design if I can do the same thing by getting more skilled with Wildfire.)

I've figured out how to do Boolean operations to subtract my part model from the mold base, but if I have a part which requires a core, I get the core and mold base as one part.

For example, imagine subtracting a hollow cylinder from a square block. Now I have a round hole in the block, but also the negative image of the hollow interior of the cylinder.

My question, then, is this: can I simply cut my mold base (from which I have already subtracted my part) into two pieces to form my base and my core without having to create a feature to remove the core from the base, and then re-create the core?

Simply put: is there a way to take one solid part (say a block) and cut it into two separate parts, so that in the end I have two .prt files?

Any help would be greatly appreciated. Thanks!

 

[jeff4136]

> is there a way to take one part and cut it into two ...

The exact steps will depend on whether you're using Foundation or have AAX, I believe, as well as personal preference. Anyway, the principle is to copy the part shell surfaces into individual part files and whack away appropriate portions there. Using Foundation this will take place within the context of an assembly and be accomplished with either a Merge (Insert > Shared Data) feature or simply copying shell surfaces and any other common (parting surfs, etc.) geometry. Hunt around. There's been a fair amount written on the subject to help get you started.

 

[LeifMasrud]

I'm not sure what you mean by either Foundation or AAX. I'm using Wildfire 3.0 with no add-on packages whatsoever.

I'm also working with solids, not surfaces. I've seen a lot of posts (here and elsewhere) regarding splitting surfaces and quilts, but I'm working only with solids.

I'm basically looking for a Boolean-esque operation (like the merge operations in an assembly) that, instead of actually subtracting material away will simply split the part along a sketched profile, or a datum plane, or something similar, giving two parts where there was only one before.

I know this functionality exists within the Mold Design module, but I was told everything that can be done in Mold Design can also be done in standard Wildfire, just a bit more manually.

I hope this clarifies my question a bit.

 

[jeff4136]

Ok, Foundation (no Advanced Assembly Extension), Solids or Surfs; no matter except for the functions used.

I don't know of a button that will split a part and create two parts. If you've already boolean subtracted a pipe from a block you've addressed the basics. I think you'll just need to repeat the process to get block_half_A.prt and block_half_B.prt.

To split the individual parts, pick an appropriate datum plane or parting surf and Edit -> Solidify.

 

[LeifMasrud]

So what I'm hearing is that I pretty much have to subtract my part from the mold workpiece, then make a copy of the workpiece (which now has a cutout in the middle somewhere), and then remove the appropriate portions of each copy by creating another feature (solidify, or cut, or whatever).

This would make things much more difficult when you don't have a simple planar parting surface, but rather one that jogs about.

Thanks for the clarification. If anybody has any easier ways to do this, I'm all ears. Thanks again!

 

[jeff4136]

By all means, keep watch. Someone that actually does this
sorta work on a regular production basis might pop up and
straighten us out. I'll go ahead and outline the flow I
think I'd use, then watch and learn.

Based on assumptions ...

_ Using Foundation all dependencies, surf copies, shared
data merges, cuts, etc. must be created in the context
of an assy.
_ More than one mold blank will be used and it (the model)
is something I ...
__ will either want to use more than one instance of but it
might be modified and I want my finished blocks to be
dependent
__ or is a model I don't want to alter, i.e. a family table
member.

... I would ...

_ Place the molded part and mold blanks in an assy.
_ Referencing them, create the parting surface as an
assembly feature (plane, nonplanar surf, quilt as
applicable).
_ Create a new part: mold_block_01.
_ Copy (by whatever means; shared data solids, surfs, etc.)
the appropriate mold blank, molded part and parting surf
geometry and perform the boolean, cut, etc. operations.
_ Create mold_block_02 and repeat.
_ Create a Simp Rep that Excludes the blanks and molded
part for drawing views, etc.

- - - - -

It's not (?) as complicated as it sounds and could be
simplified, going back to something like your sequence
tho' with lose of versatility (swapping out family table
members?), or so I tend to think.

I'll let someone that actually knows what they be talking
about take it from here. `;^)

-----------------------------

 

[LeifMasrud]

Thanks for all the tips. I appreciate it!

Here's a related question that may help to shed light on the issue. Is there a way to delete orphaned segments of a solid part? If I've completely severed some geometry by creating features, can I easily get rid of the orphaned chunk floating in mid-air?

(As in my previous question, say I wanted to subtract a thin-walled tupperware lid from the moldblank side A, where the lid's bottom surface intersets the moldblank's top. If I do so, I have the negative image of the lid as an orphaned chunk of material that's still a part of the model.)

What I've done in the past is simply sketch a cut that would wipe out the geometry. But then you actually have extranious features that don't really add information to your model, they simply clean it up.

Is there a better way to deal with these situations, or a better practice to avoid them?

 

[jeff4136]

A universally applicable method of removing disjoint
bodies involves a Seed and Boundary surface copy and a
Solidify feature.

One of the things you'll have to evaluate is the use
of 'solid' vs. 'surface' functions. If you'd simply
copied the relevant tupperware lid surfaces and
integrated them into a quilt to cut the block instead
of using a solid boolean operation ...?

I don't value a 'sparse' Model Tree. If I can get thru
a development process, struggle with some of the
geometry definitions, possibly create a dozen
'construction geometry' features to support one or two
that create model topology and end up with clean,
editable surfaces and coherent, editable dependency
chains I'm happy. A few seemingly superfluous features
may enhance the process and I'm not going to sweat a
few 'fliers'. `;^)

 

[davidinindy]

I agree with Jeff. in this case, if what you have works, then I wouldn't worry about the extra steps in the model tree.
It doesn't matter what route you take, as long as you get there.
I did mold design for 10 years, and after seeing and evaluating some of the mold design software out there, I couldn't imagine trying to do without it. It wouldn't take long to pay for itself at all.

David