How to subtract one shape from another?

[Anonymous]

I have constructed a model of a small part.  It is a bit larger than the actual part.  The goal is to 3D print a custom case that can hold a dozen of these.  The case is three solid bodies.  The intent is to "press" the part halfway into the main body of the case, and then "press" the part halfway into the cover; the case body is a couple mm thicker than two part-semi-impressions, and the third body is a cover on the opposite side.  Now the question is, given the model of the case and the model of the part, how do I go about doing the subtraction of a half-part from each of three solid bodies.

If I need to include the part as a fourth body, how would I include it in the multi-body part file I have.  I thought I could do a cut when I placed these in an assembly (remember, the part model is larger than the actual part so these is about .5mm clearance in all dimensions) but this does not seem to be an option.

A simple example is creating a cylindrical hole evenly split between two solid extrusions.

Also, when I tried to do a "place" and added a constraint, I use the XY plane, which bisects the cylinder, as the constraint "selection one", the arrow points away from the solid object I want to embed it in; when I select the mating surface as "selection two", the cylinder rotates 180° in the XY plane and now hangs out the side.

Thanks in advance

    joe

[Sergio.D.Suárez]

Can you show a picture of what you want? At first impression it seems to be a work of molds, a simple method could be to work with a solid multibody in a piece, and then by means of the tool combine, "subtract" the bodies in the solid that corresponds (remember not to eliminate the solid of cut in each operation). If you have the pieces modeled separately, you can derive the parts in the main piece file, and once the results are obtained you can create components from this main piece, I hope to be clear

Here is an example of what I said
regards!

[johnsonshiue]

Hi! It is a bit hard to visualize the case without seeing the model or an image. Have you tried Combine command?

Many thanks!

[blandb]

If I am understanding you correctly:

Take your parts and pattern them in an assembly. Next, Place your upper and lower case halves and assemble them. Finally edit one half of the case, or where the impressions need to be and use the copy object from the expanded Modify Panel.  Choose the style you want, and the part is then copied into the case half. Use the sculpt command and select the items to be removed. Below is a snap shot of a final foam piece:

[Anonymous]

Thanks.  I'll give it a shot.

[Anonymous]

I have an extruded rectangle, about 8mm thick, 25mm square.   I have a 5mm diameter cylinder I want to put in it (actually three in a row, but that's a minor detail).  So it will be laying there, in a cutout sized to it.  As I said, my model is .5mm larger in all dimensions than the real object.  So now, I have a block with half a cylinder sticking up above it.  So I will take another rectangular extrusion (ok, this is the simplified version), What I want to do is join the second block to the first, which requires that I cut a corresponding shape in this second block.  Now, if I lay this on the table upside-down, I should be able to lift the "bottom" off and see half of the cylinder poking up above the "top".  A sample of what it should look like for this simple example is attached.  I've using Inventor 2018. I show only the body and the cylinders as they might appear laying in their semicircular cut.

[Sergio.D.Suárez]

Here I send you an example so you can look to see if it is something similar. it is a base multibody file, it is modified from there, then the assembly and its components are updated from the multibody

Regards!!

[JDMather]

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@Anonymous wrote:

... I've using Inventor 2018. ...

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Are you using Inventor 2018 standard or are you using Inventor 2018 Professional?

[blandb]

My apologies, I spaced out the multi-body aspect and was using just a part file that was a pattern at an assembly level to create the impressions.

[blandb]

If you have your multi-body case, and you have performed the "Make components" option, you should have an assembly. Case component and foam or whatever the cushion is. If you place that assembly into an upper level assembly, then place your piece part into that assembly as well. Constrain and pattern however many instances you want. You should be able to do an in-place edit of the cushion part. Use the copy object to bring the patterned instances into your cushion as a composite, then sculpt the included surfaces out. Using a composite will be a surface that is adaptive to the main assy. If you shift your pattern, then the cushion will update. Finally, you can use thicken/offset and cut away the desired amount from your cushion by selecting the surfaces you want to remove. This will give you a gap around your part where ever you want it. Draw back is, this will not appear in the multi-body solid.ipt that the case was created from. When you use your cushion.ipt file that was created from the make components in a drawing, it will have the impressions in the part. Hope that gives a workflow that you can use.