split or cut a single body into multiple bodies.

[Anonymous]

I would like to know how to take a solid body and through splitting and extruded cuts turn it into multiple bodies. this is very easy to do in solidworks. I use inventor because for mold design it is more robust and when doing cavity/core functions i can retain the toolbody. that is a life saver. many times though i will need to split a part across a plane but only seperate a couple details. in solidworks you can select which features get cut and which ones don't and you also have the option of combining features together after a cut. The easiest example i could give would be that if i take rectangular block and cut a ring though it i will be left with a block that as a hole in it and also a cylinder inside of that hole. In solidworks this would automatically be turned into 2 solids. In Inventor it will still be counted as a single solid. 

Please keep in mind that this was a simple example and so i don't need to be told how to extrude a hole and redraw the pin as a new solid. There are many instances where i create a cavity and then need to turn certain areas into core pins with that feature and so in solidworks i just do a circular split through the block and now i have a new solid with that feature on it. So, the actual question is; can Inventor do this or not? currently I just export my block, fix it in solidworks and then re open in Inventor. The pic i included is an example of a detail that i extruded a ring through to turn one of the details into a pin. unfortunately it is still being seen by inventor as 1 body when it clearly should be 2 seperate bodies. 

[jhackney1972 · Accepted solution]

There are a couple of ways to accomplish what you want in Inventor if I understand your question correctly.  It may not be the same command(s) as Solidworks but it get the job done.

Take a look at the screencast, I hope it helps.

[johnsonshiue · Accepted solution]

Hi! This topic has been discussed repeatedly in the past, particularly with SWX users. The reason why this particular workflow is not straight forward in INV is because of a fundamental difference between INV and SWX. INV supports so-called disjoint lumps. For example, if you create two separate extrusion apart from each other, they can still be one solid body, though they are not merged together. Certainly, Inventor also supports multiple solid bodies. SWX on the other hand, only support multiple solid bodies. There is no such thing called disjoint lumps in SWX. Each piece of separated geometry is a different body.

INV could support the result you are looking for with a separate command. Or, you can use the workflow suggested by John. But, it would not be part of any existing command or feature. It is because it could be confusing. The user would need to decide if the result should be disjoint lumps or separate solid bodies.

One may ask why disjoint lumps are needed. It is a very powerful tool actually. For example, when you try to create a massive pattern of geometry, the disjoint lumps help make the patterning process very quickly and keep the data as compact as possible.

Many thanks!

[TheCADWhisperer]

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@Anonymous wrote:

.... So, the actual question is; can Inventor do this or not? .... 

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The process is essentially identical in both Inventor and SolidWorks - so I don't understand the issue (I use both).

Can you attach example *.ipt and *.sldprt files here?

[Anonymous]

This part has an upper half and lower half, formed around a part. this is
supposed to represent a cavity/core mold feature and there should be a core
pin to create the internal features of the part. When I split the mold into
2 parts the top half is still showing up as 1 solid even though is clearly
is 2 separate solids that are not touching each other. In SWX this would
have showed as 2 solids and then I could easily attach the round cylinder
to the bottom half and create the pin from there.

[hosford]

If you use the split tool you can make 2 solids from your model

[Anonymous]

Actually, i did use the split function. I've included a sample file. you
will see that the top split has 2 parts in it but still counted as 1 solid.

[hosford]

Couldn't find your file.

But if you have 2 solids in one part file, you can use the make components command to generate an assembly and associated details.

[Anonymous]

That is a very good explanation of why it doesn't. It makes sense. Surely there must be a way to create the 2 parts though. I am including a sample part to illustrate what i'm trying to do. After cutting this part into 2 pcs, the top half has a cylinder in it that should be considered a separate solid and I would like to attach it to the lower half of the part. 

[Anonymous]

Sorry, the files didn't upload for some reason. 

[TheCADWhisperer]

The SolidWorks file is useless as there is no feature history.

Sketch1 in the Inventor file does not have any dimensions?

I can show you how to do this in both SolidWorks and in Inventor.

Work Plane1 is not needed - not in Inventor and not in SolidWorks.

[hosford]

I imported your solidworks file into inventor, then utilized the make components command, selected the 4 solids and made an assembly with 4 individual parts.

if you modify the original solid that has the 4 solids in it your assembly and details will update.

[Anonymous]

Here is the SWX part with features. When i split the part i have the option of deciding what solids are created. This is the part i am trying to get INV to make

[Anonymous]

Thanks for your offer to help. I would really appreciate learning how to do this in INV. as for sketch dimensions, they are irrelevant on this part. i only made it to illustrate the problem I am having with the split tool. I sent you a similar solidworks part that illustrates how easily it works in that program. Normally i would just use SWX and move on but I actually like using INV better and when i do combine features, INV lets me keep my original part which is great when designing molds. In SWX when splitting you have the option of deciding which features get cut and which do not. this is really handy.

[hosford]

You have everything there you need.

if you are wanting to use the solid works file and import it into inventor, then do so, you will end up with a part file with two solids, in that part file use the make components command, this will make an assembly file and when that file is saved you will have individual solid part files that you can detail easily.

[Anonymous]

Thanks for trying to assist me but that is not what i was asking. I am attaching a couple files that will illustrate my problem. The SWX file is what i am trying to make. 

[TheCADWhisperer]

I noticed that the technique you used in SolidWorks removed your toolbody?

Back in a few minutes with a couple of different solutions.

Part Gone?

[Anonymous]

That is correct sir. In SWX i used the combine/subtract command and there isn't an option to keep tool body. That's actually why i started using inventor so much. I actually use the tool body for creating multiple reverse images for electrodes and INV works great for that. If there is a way to keep the toolbody in SWX that would be helpful to know as well. thanks for your help. 

[hosford]

https://knowledge.autodesk.com/community/screencast/7c044ad2-1ec4-46af-b9af-8220f0aa0b90

[TheCADWhisperer · Accepted solution]

OK, here are three different techniques.

The first technique assumes that you might have much more complex parting lines than this simple example and that you have Inventor Professional with the Mold tools.

The second technique assumes that you don't have Inventor Professional with the Mold tools and that your parting lines are relatively simple.

I didn't demonstrate the third technique as it is really just a variation of the second technique - but I did attach a file example.  The key is that Inventor supports disjointed lumps (which SolidWorks does not) which can sometime be very useful, but in this case detrimental to our Design Intent.  So the parting line between core/cavity Split surface should only split what you actually want to split.  (Workplanes split everything.)

I didn't demonstrate a forth technique using Derived Components that I really like in certain situations (keeping the part and tooling in different associative files).

Screencast will be displayed here after you click Post.

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