Subracting one solid from another dumbed down.

[stuart.homer]

Hi , this is a bit of a strange one that i would have no problem doing in NX. We basically fill our product with glue and i want to create a model for the actual glue so i can measure the weight of our product accurately in the model. I was going to export a STEP file of the product , create a block in an .ipt , import STEP file and subract , then trim up the remainder with trim planes . It would seem though Inventor seems to retain the assembly information when importing the STEP even if you select 'reference model'. Can you not just remove all parameters and detail from an assembly model in inventor ? How would i go about doing this procedure ? 

[JDMather]

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@stuart.homer wrote:

I want to create a model for the actual glue so i can measure the weight ... How would i go about doing this procedure ? 

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Derive Component.

All will remain associative - so if you change a part or position the Derived "glue" part will automatically update.

Attach your assembly (or dummy assembly if proprietary) here if you can't figure it out.

[stuart.homer]

Hi JD ,

Thanks for the reply and i cant really post the model due to IP. The question is actually how do i create the actual glue , ie , how do you subract an assembly from another solid. See image - i need to fill the whole cavity up to the three internal faces in the middle . I cant believe its that difficult but im pretty new to Inventor.

 

[RNDinov8r]

To subtract an assembly from a solid, you can use the sculpt command. Start the new part. Exit the Sketch. Select Derive Components, insert said assembly, as a surface - not a multibody solid. Sketch the new part, "glue", then use the sculpt command to have only the "glue" remain. YOu can hide the visibility of the surface for clarity.

[JDMather]

I understand the question.

Attach dummy assembly here.

Or do you need for me to demonstrate that too?

There is a second technique, but it would be best to have a representative assembly so that I do not have to demonstrate both techniques.

[imajar · Accepted solution]

What you are describing is a perfectly good way to do it, although maybe not optimal in the inventor world (try exporting to .sat instead, then you can reimport as a single part, combine bodies and all that).

But, let me suggest instead:  Open a new part, click the manage tab, click on derive (in the insert section of the tab).  An open dialog appears, navigate to your assembly and open it.  Then you have a bunch of options.  Set the "derive style" to merge bodies.  From here, you will have the imported geometry hopefully as a single body that you can do subtraction operations on (using the combine command).

Alternatively, create a new empty part within your assembly, and use the copy object command to copy selected bodies from other parts into the new empty part. . . if that sounds like more what you want then google it or let us know and we can explain it more.

[johnsonshiue]

Hi Stuart,

I am not sure why you need to export it. You can do it using Derive or Copy Objects (3D Model -> Modify -> expand the panel). Please share an example here. It should be fairly easy.

Many thanks!

[stuart.homer]

Hi ,

Thanks for the replies all , i think my lack of inventor knowledge is the issue here and being a bit old school.

I have achieved what i want but i doubt very much it was the best way. I derived the assembly with merge as ajarrett suggested and created a basic block in that part and combine subracted the derive , added trim planes and trimmed up the whole thing. I had some issues with it not trimming properly , so exported to SAT , opened that with multi-body and direct model deleted the untrimmed faces. RE-exported to SAT and RE-opened as ipt multi body. Edited the material and dyed section and there you go.

I need to look at the derive command in more detail when i get time and get some proper Inventor training - We were booked in but lockdown got in the way.

 

[JDMather]

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@stuart.homer wrote:

....so exported to SAT , opened that with multi-body and direct model deleted the untrimmed faces. RE-exported to SAT and RE-opened as ipt multi body. Edited the material and dyed section and there you go.

I need to look at the derive command in more detail when i get time and get some proper Inventor training. 

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Sounds like a complicated round-about way of getting there.

Derive as surface body and Sculpt (“flood fill”) your desired body.

All will be associative.

I will make wager that your trainer will not know how to do this.

[stuart.homer]

Thanks JD ,

I knew there would be a better way. We are talking about a bit of a redesign of this product so ill try your way after that. At the moment i don't mind its not associative. I have 28 years in NX and about 2 solidworks and 1 Inventor so in my head i know what i want , its just how you go about it in the Inventor interface. In NX you can just export and unparameterise the model , model a cube and subract and trim.

I do suspect however that your method is the more correct way of going about it.

Yeah , im not going to get trained on that in a 2 day session , so im not having a bet with you 🙂

Stu.