Making a cut from my assembly

[sps_cad_guy]

I have attached a couple of screen shots trying to show what I need to do.

I have an assembly of 6 pieces of tubing that have overlaps in material.

I am needing to make cuts, in the parts, from my assembly level.

How would I go about making my cuts in each part from where the cutting circles would be located in the assembly?

Thank you so much for your help.

[graemev]

If you can generate a skeleton frame of the centerlines of the tubes instead of an assembly of the tubes themselves, Frame Generator might be a preferred method, simply using the Notch tool on the tubes.

[sps_cad_guy]

Ok, thanks.

I'm really at a loss as what you mean by this, but I will research this area and see if I can get this taught to myself.

I appreciate pointing me in the right direction.

[graemev]

Take a run through the Frame Generator tutorial.  At the very least you should be able to see the basic concepts of skeletal modelling.  If you need further help, feel free to come back and ask.  (I'm inclined to teach a man to fish, not give him a fish.) 

[JDMather]

The Frame Generator would be the easy way, but -

you could also edit each part in the context of the assembly

Copy Object the trimming face as surface body

then Sculpt or Split.

Fairly easy to demonstrate with actual Inventor assembly files.

[sps_cad_guy]

Thank you very much.

I went through about a dozen and a half videos of Frame Generator tutorials, but found none doing what I need to do.

I did find a video on the Copy Object and using Sculpt.

This is slow and tedious, so I am going to continue to try and find a tutorial that fits what I'm trying to do.

Thank you again for your help.

[sps_cad_guy]

I have come across another problem I am having with this assembly.

I have my tubes cut out using the sculpt.

Now, I have two seperate planes, one at the bottom and one at the top.

How do I trim the pieces of tubing above the top plane and below the bottom plane?

I tried both the sculpt and split, but I couldn't select the planes.

When I tried the trim, I got an error saying The selected component has no surfaces.

[JDMather]

Is the plane at the part level or the assembly level?

Couldn't something this simple be done as multi-body solids and the assembly pushed out, or is there more complexity than you are showing in your image?

Can you attach a real Inventor assembly?

In the real world - will the parts be cut before or after assembly?

[sps_cad_guy]

The story on this project is:

I was given a photograph and asked if I could draw this up and program it for our tube laser for the big shots to show off our tube laser's capability.

Normally, we only do parts, so my experience with assemblies, especially with Inventor, is very limited. Also, I have basically taught Inventor to myself, so a good portion of the things I read on here, such as multi-body solids and the asssembly pushed out, are Greek to me.

I've attached my assembly and part files to this.

Thank you very much for your help.

The planes are at the assembly level.

[sps_cad_guy]

Yes, all cuts will be done on the tube laser, before any assembly.
Thank you.

[JDMather]

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@sps_cad_guy wrote:
Yes, all cuts will be done on the tube laser, before any assembly.
Thank you.

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OK, so these will not be of any use to me.
I think this problem will be trivial using multi-body solids technique.

Are the laser cuts always perpendicular to the cylindrical surface, or can you really cut like this image from one of the parts you attached?

[sps_cad_guy]

Yes, the laser cuts will be perpendicular to the surface. The programming software will do that automatically.

Thank you, I will look into videos on using the multi body solids.

I do appreciate all the help.

[JDMather]

That is what I thought.

So this is how I would do the model.

Extrude tube OD as surface bodies.

Trim the surfaces.

Thicken (New Solid for each after first).

Manage>Make Components to push out the individual parts and assembly.

[sps_cad_guy]

Thank  you.

I will see what tutorials I can find on all of this and see what I can figure out.

Thank you again for your help.

[sps_cad_guy]

Ok, I hate asking this, but are you saying to do this to the parts I have already created, or delete everything and start back over?

I'm not finding any very useful videos to learn all this from, and just really don't know where, or how, to start.

[JDMather · Accepted solution]

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@sps_cad_guy wrote:

.... start back over?....

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I started over.

See attached Master file.

It might initially look more complicated than it really is, but if you drag the red End of Part marker to the top of the browser and then down step-by-step, you will see that it was quite easy.  (Spacebar repeats commands.)

This was my first attempt.  Now that I understand the geometry - I think I could still significantly simplify the process, but I have to move on to other work.

BTW - you should install Service Pack 2.

[sps_cad_guy]

Thank you so very much!

I had started on doing it over again, and looking at how you did this,

it's making more sense the further I get into it.

Again, that you so much for  your help.

[WHolzwarth]

Here's another approach, with as few notches as possible. (2014 file)

Walter

[JDMather]

Ah yes, I cut some that did not need to be notched (unless that was the design intent).

Good catch.