Flattern tube wall for fishmouth CNC plasma cut

[giorgio.demurtas]

Hello,

I would like to plasma cut the red pipe so that it sits on the red tube. I need to project the outer surface of the red tube on a flat plane, so that I can use it as X-Y coordinates to run the plasma cutter (to be built, so far I have made this CNC router: http://www.ingdemurtas.it/automazione/cnc/ ), or print it on paper to wrap around the tube as a template.

The drawing below was made in the modeling workspace. I read here that F360 can flattern only sheet metal, but how do I create a tube in the sheetmetal workspace?

[beresfordromeo]

hi @giorgio.demurtas

I hope I can help you. Which body do you wish to flatten and plasma cut, the red or the green?

[giorgio.demurtas]

The green. (sorry, I have a typing mistake in the first message. It seems I can't edit it...can I?)

The correct question is:

"I would like to plasma cut the GREEN pipe so that it sits on the red tube. I need to project the outer surface of the GREEN tube on a flat plane, so that I can use it as X-Y coordinates to run a CNC plasma cutter, or print it on paper to wrap around the GREEN tube as a template."

[etfrench]

My Google Fu isn't working tonight, but there are several threads on the forum detailing how to create pipes and cutting templates using the Sheet Metal workspace.

Basic concept is to draw a 359 degree arc. Create the first flange using the arc. Extrude (not Press/Pull) one side of the slot a small amount (Less than one degree).  Align this sheet metal pipe with the other pipe (probably best done when drawing the original arc). Use Combine|Cut operation to remove the unwanted section of the sheet metal pipe.  Flatten the sheet metal pipe using the small extrusion as the base.  You can project the flattened sheet metal part to a sketch, then save the sketch as a dxf.

[beresfordromeo · Accepted solution]

hi @giorgio.demurtas

I have recorded a screencast for you with a possible method for this. 

It is no the same as the one described by @etfrench but you will get the idea.

[beresfordromeo]

No problem. You can edit a post if you click on options on the right.

I have recorded a screencast for you above. I accidentally replied to @etfrench sorry about that .

Let me know if you need any further help with it.

[giorgio.demurtas]

It worked well, thanks for help!

For other newbie which might came across this post, here a few tips from my experience:

- to make the sheetmetal flange, the sketch profile must be open (a closed circle won't work!)

- It must have a portion of straight line, which will create a flat portion of the flange. You must have this flat portion to be able to unfold the bends.

- Once unfolded you might find that the width of the sheet metal is smaller than the circumference of your tube. This is because F360 takes into account that the metal stretch/compress when bended. To reduce this, you need to set the thickness of your sheet metal to a small value (I used 0.8 mm).

[beresfordromeo]

You are most welcome.

Good observations about the method and very helpful to others  that you have taken the time to add them. 

On the thickness of the material, it could be that you can also allow for this using bend override. I don't know the sheet metal environment very well so hopefully someone could help us with some thoughts on this. 

Best of luck with your project.