Creating flat drawing of tube

[Anonymous]

Hi everyone,

We recently purchased a 4 axis plasma table. We are hoping to be able to cope the ends of tubes utilizing the 4th axis. The CAM program supplied with the machine wants a flat drawing (which it will then wrap around the tube) of what will be cut. 

My first thought was to convert the tube to sheet metal and then create a flat pattern or unfold it. But every time I convert to sheet metal it converts the end face of the tube, not the surface around the tube. The picture below is a very basic cope on the end of a 1 inch tube. The highlighted face is what it always ends up converting rather than the entire outside of the tube. 

[SEANT61]

Clearly, diligence and Inventor have a lot to offer. 

[JDMather]

I just realized that the Delete Face step can be eliminated (at least for this tube) by using Thicken-Intersect instead. (see attached)

[Anonymous]

That is really cool! We already have all of the tubes modeled for the car that I am helping to build, but I will pass it on to other design teams to play with. 

[Anonymous]

kind of hard to tell what is going on. It looks like you used thicken on the inside face and used the Join selection. Is that right? 

[JDMather]

---

@Anonymous wrote:

...used the Join selection. Is that right? 

---

No, that is not correct.

I used the Intersect option - perhaps the most overlooked tool in Inventor.

Join would not change the part at all in this case.

Cut would leave only the ends.

Intersect removes the non-intersecting portions of the ends because they do not, well, intersect with the Thickened material from inside - out.

[Anonymous]

I must have accidentally changed it to Join when I was looking at it. Was in a bit of a rush this morning. 

Definitely haven't had a use for the intersect tool until now. Seems like it will be useful for most of our copes until you exceed a certain angle, at which point your first method should get the job done. 

[S_May]

hey @Anonymous, what is your answer to all the good Solutions...?

[Anonymous]

That is a good question. There are several good options. I think that my choice will have to be the first screencast posted by JDMather as it works with all of the models we already have, works with any angle of cope, and takes into account that the cutter will always be perpendicular to the tube. 

The iLogic controlled one is really cool too! But would require us to use that model to redraw every tube on all of the projects that use tube frames. Potentially very useful for next year's vehicles since they are redesigned each year. 

As much as I love Inventor (my personal go to), design teams and other students often bring me drawings in Solidworks instead of Inventor. If anyone is interested, I will be creating a similar thread on the Solidworks forums to see if we can get the process figured out in both software packages. Seems like it will be a very similar process, but Solidworks isn't playing well with making the tube a sheet metal part. It asks for a lot more information than Inventor does, and I'm sure I probably have at least one thing set wrong. 

Thanks for all the help everyone! 

[SEANT61]

---

@Anonymous wrote:

. . . . with any angle of cope. . . .

---

What does "angle of cope" imply?  Any Tube/Tube connection other than a perpendicular "T" juncture will need that secondary processing shown in my first screencast, and explained in the linked thread.

[Anonymous]

Well, a perpendicular T (like the example files) are a 90 degree cope. Like in the second part of your screencast, the upper tube is at a different angle (somewhere around 30-45 degrees?). 

Without any narration, I couldn't tell what certain steps accomplished. Especially since you are using AutoCAD for 3D modeling instead of Inventor. I very briefly touched on 3D modeling in AutoCAD in a class 5 years ago. But I don't remember much about how to use it well. 

What I meant by choosing the first screencast by JD instead of the second is that his idea of using the thicken tool and the intersect option will only work up to a certain angle before it starts placing/removing material in the wrong places. The first method of deleting the outer face and then thickening the inner won't, or at least to a lesser extent. 

[SEANT61]

I can only provide AutoCAD based geometry, hence my screencast and DWG file, but the geometry does demonstrate an issue that any software will need to address.  Anything other than a perpendicular "T" juncture requires the  removal of additional material for a clean fitting connection (i.e., no post CNC grinding).  

That additional step is explained in the linked thread - essentially after thickening the inside wall to the outside, the outside wall must be thickened towards the inside.  The Intersection of those two solids creates the necessary mating condition.