3 Axis Parting Line for Surface Cut

[Anonymous]

I need to design two clamp blocks (top and bottom) that have a gripping cavity that matches a imported step file of a tube. I have used "combine" before to cut a surface contour for a tube that only changed direction in 2 axis. I dont know where to start when you have a tube that changes in all 3 axis. I need the clamps contour to match the split line of the tube so that the tube can be inserted into the clamps. I attached a example iam file for what Im trying to do.

[Marco.Takx]

This is only a indication of how yoy can create clamps for something like this.

I first used your block (Part3) and saved that as Clamp1 and Clamp2.

I placed those Clamps into the assembly and constraint them on a place around the tube.

Then I made a copy object of the tube within Clamp1 and Clamp2

After that I placed on bould sides of the tube a workplane with a offset of 0.

Then I used a sculp for the tube and bould workplanes so the tube becomes massieve.

Finally I did a cutout combine.

See the files attached overhier so you can see it yourself.

Use your Tube.ipt fiel for this assembly.

Good luck!!! 😉

[Anonymous]

Thanks for the reply. I am familiar with using the copy object and using combine to cut the surface. However I need to take this a step farther since the tubes centerline changes in all 3 axis. The probelm with the clamp block you attached is that you will be unable to insert the tube into the clamps (see clamp1 picture). The parts cavity parting line should look simliar to picture2 and mating part picture3.

[WHolzwarth]

This could be a task for Core-Cavity-Splitting in Mold Design.

I came so far:

But during the preview, Core-Cavity-Generation failed.

Autodesk, improvements are needed.

Walter

[Marco.Takx]

Hahaha I see that Walter was on the same way.

I thought your challange was my first solution but hier is the second one 🙂

See the model in the link below.

I hope this is what you want.

http://a360.co/1GeUhyY

Good luck!!

[WHolzwarth]

Not good enough, Marco.

There are different silhouette curves on opposite directions for most surfaces. 

[Marco.Takx]

Hè Walter. I know that the model is not perfect, but this is only a model to sent him in a possible direction. 

[JDMather]

This might give you some ideas (see attached).

Now let me take a look at your example.

[WHolzwarth]

Here we go.

I've used a simplified tube, where some of the external fillets were deleted. No problem for a clamp and even better for this task, but a mold should be able to handle parts fillets as well. (Autodesk, are you listening?)

It's been no straightforward task. 2016 files in Zip, EOP in tube-simplified.ipt needs to be pulled back down again.

Walter

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[Anonymous]

The end result looks like what I am after. I'm having a hard time following how it was done though.

[Anonymous]

Although this looks like it would work as a clamp, the pink face doesn't look right to me. Its should follow all three silhouette curves of the tool body. Like how the example JDMather posted.

[WHolzwarth]

IMO it's looking good.

I've made a Draft analysis of the tube with very low limits (-0.1° to 0.1°). Then you get a very sharp color change at the silhouette lines.

As can be seen , the parting faces are placed well at the silhouette.

Walter

[Anonymous]

Its not what I'm used to seeing but I agree it does look to be split correctly. However why is the resulting surfaces getting abrupt changes?

[WHolzwarth]

That's because I deleted this face in the simplified tube. It's a transition patch between two cylindrical sections.

If you place axis for both cylinders, then in ideal conditions they would have an intersection point. You can't get that with your original tube, therefore parting faces need to have a jump.

But that doesn't matter. Generally it's best if the whole tube is clamped only at two or three short regions.

That's cheaper and better. You can choose these regions as you want from the whole geometry.

[WHolzwarth]

Hmm. I've looked again at the original tube.

An intersection point can be found between both axes.

I'll try a simple sample.

[WHolzwarth]

Simple sample looks ok.

Perhaps Autodesk QA can comment about the differences on the original tube.

[Anonymous]

JDMather, this looks like what I am looking for. Is there any way you have a step by step video of what you did to get the end result?

[JDMather]

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@Anonymous wrote:

JDMather, this looks like what I am looking for. Is there any way you have a step by step video of what you did to get the end result?

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I am really busy this week into next week.  Not sure when I will have time to create a video.

I think I have a paper on the steps, but Inventor has changed a lot since I wrote the paper (now supports mult-body solids) and it might confuse more than help.  Let me see if I can dig it up.

Initially it seems quite complicated, but after going through the process a couple of times - a robust and general technique is developed.

This one is important and unique enough that I am motivated to do a video, I just need to find the time.

[WHolzwarth]

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JDMather schrieb:

I think I have a paper on the steps, but Inventor has changed a lot since I wrote the paper (now supports mult-body solids) and it might confuse more than help.  Let me see if I can dig it up.

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Here it is, starting at page 34. Jeffrey did it in 2008:

https://forums.autodesk.com/autodesk/attachments/autodesk/78/547673/1/ML205-1P%20Mather.pdf

It's been state-of-the-art in 2008, but meanwhile Inventor can do better. See pictures. The blue regions sign undercuts.

I'm convinced  that Jeffrey will provide improvements with a renewed sample.

Walter

[Anonymous]

I've been working at this some. The process that has been posted seems more complicated than it needs to be. I'm thinking of taking a different approach. I have made it far enought to where all I need to do is use the split command to split the two clamps with the silhouette curve that I made. I would think that I should be able to create a boundry patch with the silhouette curve I created but I keep getting a error message that says the path has discontinous segments. I would think that after I get this surface created that I could use it to make the split and be done with it. What am I doing wrong when trying to create the surface? See attached file.