Need help to draw tubes running in different planes

[Anonymous]

Hello folks,

I hope everyone is safe and doing good. 

I need help with Inventor in making out tubes (1.5" od) which are running in different planes. 

So I have a drawing as shown below and we need build this in our shop. I need to make drawing for tubes so shop guys can bend this. Please not the tubes are not allow to welded to make them bends. They have to be one piece. 

So far I have made the lower header tube and top plate as shown in snapshot below. I have also made tubes in bottom header as they are similar up to that point beyond which they are running at different angle to match with top plate holes.

Is there anyway I can make this faster in inventor.I can make the tubes one at a time which is not preferable as It is very time consuming. These are 260 tubes so 260 different parts I have to make. 

I would appreciate if anyone can help me and guide how can I do this. 

Thank you in advance

Regards

Stay safe

Chints

additional view of this project

[CGBenner]

@Anonymous 

Use Sweep to make one, and then Pattern it as many times as you need around the OD.

[Anonymous]

Hi @CGBenner 

Doesn't work that way, the one made with sweep will remain same in pattern at all 260 places. as you can see each tube will be different. 

[CGBenner]

@Anonymous That was not immediately obvious to me.  Hard to tell from your image.  So no, that won't work. 😕

[Anonymous]

Hi @CGBenner 

Apologies for not providing sufficient information.

I have included few more view for clarity.

[johnsonshiue]

Hi! Please share the files here. Forum experts can help take a look and provide guidance.

Many thanks!

[Anonymous]

Hello @johnsonshiue 

Attaching part and assembly files for anticipated solution.

Feel free if anything else is needed.

Thanks so much

[imajar]

How are you going to convey the information to the shop?  Will you be making a drawing for each tube?  (my sympathies if you do)  Or export individual tube models to a bending software?  Or do you need the model to just be one part, you put on some general dimensions and rules and the shop figures it out?

[Anonymous]

Hello @imajar 

Basically I am hoping to make this virtually and then I will make drawings for tube and if they differ in one or two parameters I will make a table for the shop guys. 

I'd appreciate if you share any similar experience you might have and suggest any efficient and productive solution.

[imajar · Accepted solution]

What a fun problem!  Try the workflow in the attached part, I don't have 2021, so I was only able to view your part.  This method only works if the to and from points have the same circular pattern and diameter, and the ends are perpendicular.

First step is to create the bends and pattern them along the intersection plane.  I do this by projecting 2d sketch points to the intersection plane to a 3d sketch.  Then, select those points, right click and convert to center points, then create one bend and use a sketch driven pattern to pattern all the bends.

The extrude the lower part of the tube, using "to next" termination and circular pattern with the "adjust" option.  Repeat for the upper part of the tube.  Hopefully that makes sense!

[Anonymous]

Hello @imajar  

Thank you so much, that helps a lot. Actually to and fro point have different  diameters but I figured out a way how to carry on this further to make it work.

Again thank you for your help.

Kudos @imajar 

[Anonymous]

Hello @imajar 

this is how wanted it to be eventually. This is just part of it I've to go long way in this. 

Again appreciated your help.

[johnsonshiue · Accepted solution]

Hi! The files are still incomplete. Based on my understanding of your design intent, I guess you would like to create a series of pipes going in a particular direction. Here is my 5 minute attempt. Is it similar to what you were looking for?

Many thanks!

[Anonymous]

Hi @johnsonshiue 

Yes you also nailed it, different way though getting same result. 

Thank you.

[Anonymous]

Hi @imajar 

Hope you doing great.

Hey I just wondering how did you do the following step in the problem. 

 " I do this by projecting 2d sketch points to the intersection plane to a 3d sketch."

I was trying to make this on my own and I am stuck at this step.

Appreciated your help.

Thanks

Chintan

[imajar]

Thats not fair to ask me what I did a couple weeks ago 😁

Oh, lets see here.  What did I do. . . .

Looking at the sample file from my post, it looks like I created a new 3D sketch and used "Project to Surface" command, select "Work Plane 3" in the faces box, and select all the points in Sketch14 for the curves, then click OK.  That will project the points from sketch 14 onto work plane 3.  

Let me know if that answered your question.

[Anonymous]

Hi @imajar 

Hey that was good one!! 😁

Yea that helped me. Thanks for quick response. Cheers!!