Notch of a curved pipe

[cinim]

Hi,

I'm trying to notch a curved pipe with another pipe and its giving me many problems because I can't select it. What can I do to work it out?

Thank you.

[cinim]

and another small question, is there a way to make the frame one whole body, apart from the beginning?

[JDMather · Accepted solution]

1. Copy Object as Surface cutting object face and Split part or Sculpt

(Attach the two parts and iam if you can't figure it out - don't need the entire assembly).

2. Derived Component combine.

[cinim]

I couldnt do as you said in the first part, because each pipe is one separate body and you can't edit them. I tried combining them then doing it aswell, but I can't for the same reason.

[JDMather · Accepted solution]

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@cinim wrote:

I couldnt do as you said in the first part, because each pipe is one separate body and you can't edit them. I tried combining them then doing it aswell, but I can't for the same reason.

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You don't understand my solution because I didn't supply enough detail.
Attach your files here.

[cinim]

thanks so much, because I was stuck there in my thesis and i need it get proper results from ANSYS

I hosted the file here: https://www.yousendit.com/download/UFh1SkhUY1NCSnBFQlE9PQ thanks once again.

[cinim]

Mr Mather, I kept on trying because I don't agree on the easy way out, and I managed to trim it or split it, but how do I delete the unwanted parts of the tube?

Thank you for your guidance.

[Dennis_Jeffrey]

The Split command has options to Split AND delete.

See below:

[rdyson]

Surface>DeleteFace>Select Lump

Might be what you need

[cinim]

First of all thanks for the reply, any help is appreciated

I tried doing that, but it seems that still the pipe won't really trim. the construction lines are perfect and everything, but when i open the pipe alone, it is still as it was before.

[cinim]

thanks for the reply. that command seems only to delete the surface, whilst I need to delete a piece of the body. is there a similar command for a solid please?

[Curtis_Waguespack · Accepted solution]

Hi cinim,

Use this option, as rdyson mentioned:

I hope that helps.

Good luck with all of your Inventor pursuits,

Curtis

http://inventortrenches.blogspot.com/

[Dennis_Jeffrey · Accepted solution]

If done correctly with the selected options, the Split tool works. See below:

If I open the trimmed tube, this is what you should see before the surface is turned off. 

[cinim]

thank you gentlemen, your kindness is really appreciated. I managed to do it.

If i may, can i ask for one last favour. Could someone guide me to how I can combine each frame into one complete structure please? That would be very helpful when converting it to ANSYS.

For future reference, if someone needs to here are the steps:

1. Select the part you want to trim, and "copy to construction" found under surfaces

2. there should be a folder named "Construction". Double click on it

3. Double click "Copy objects" and select the pipes you want the part to be trimmed around. Make sure you select surfaces

4. Finish Construction and go the Model Section. Double click on Split, select trim solid and trim as needed

5. To delete extra parts, go to "Delete face" found under Surface, and make sure you select lump

That should be all.

[Dennis_Jeffrey]

You are doing way to much work...

1. In the assembly file, edit the part you want to trim.

2. Select Copy Object from the Model tab

3. In Copy Object with Surface option selected, select the Trimming face of the other part.

4. Select Split, then select the Surface created in step 3.

Use these options (marked in red) to trim the solid tube.

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@cinim wrote:

thank you gentlemen, your kindness is really appreciated. I managed to do it.

If i may, can i ask for one last favour. Could someone guide me to how I can combine each frame into one complete structure please? That would be very helpful when converting it to ANSYS.

For future reference, if someone needs to here are the steps:

1. Select the part you want to trim, and "copy to construction" found under surfaces

2. there should be a folder named "Construction". Double click on it

3. Double click "Copy objects" and select the pipes you want the part to be trimmed around. Make sure you select surfaces

4. Finish Construction and go the Model Section. Double click on Split, select trim solid and trim as needed

5. To delete extra parts, go to "Delete face" found under Surface, and make sure you select lump

That should be all.

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[cinim]

you made it sound much more easier, heh 🙂

if i may ask another question, how could i combine all the frame members into one whole body, i.e. having 1 frame and not many separate tubes.

thanks.

[JDMather]

If you had attached just two part files involved and assemble iam here instead of the entire assembly on a third party site  - I would have shown you the easy way with your parts.

To combine your assembly into one part use the Shrinkwrap tool (see attached).
I suspect you want to delete the associative link (see image), but you could always do that later - you don't have to do it now as indicated.

[cinim]

just want to thank you all for your invaluable help. I finally managed to construct the frame as desired. Now i can move on to ANSYS and start banging my head there.

cheers.

[JDMather]

Why not use Inventor for the analysis?

[cinim]

my thesis supervisor is very keen on ANSYS as he suggests it gives better results, and since he's the one correcting the dissertation who am I to disagree? 🙂