Create a Flat pattern

[aeronerd]

Hi,

I am trying to create a flat pattern of a tube with copes in it.

When i select the flat pattern command it works without errors and opens another window. But instead of it being flat it is still the round tube.

What am i doing wrong?

[davebYYPCU]

The tube needs an open seam cut into it.

Might help...

[aeronerd]

Thanks. I have done that.

I followed this tutorial.

https://www.youtube.com/watch?v=PwiYHXiM_wk

[davebYYPCU]

Nope, has to be an open gap, not a surface body.  Extrude cut from the angled lines in the sketch.

Did you Press Pull the coping cut, like he did, the material has to have perpendicular edges.

He used the Press Pull and Split face for the bits to cut / remove.

Hint: this work is better done with surface tubes, Thicken, then extrude cut the seam.

Might help….

[aeronerd]

Thank you for your help.

Yes. I have Press Pull and Split face on a lot of tubes for this project. I should have tested this earlier.

I am only a beginner.

I don't totally understand your solution. Do you mean doing it like this example?

https://www.youtube.com/watch?v=llRj1KQxhiI

[davebYYPCU]

Ok, the first video has a pie slice shaped cut, the second uses a rectangle, and looks like he didn't have any grief, without the Press Pull effort on the coping cuts.

When a Flat pattern has non square edges you end up with a top and bottom outline that are not identical.

If you have cut the gaps in the model, and you can't get a Flat Pattern, will need you to File > Export it.  Attach it to the next message.

Might help...

[aeronerd]

See attached file. This is just one section of it.

[davebYYPCU]

Ok, that body belongs to a Base Feature - (Timeline removed if there ever was one - not in either video)

Yes it was converted to Sheetmetal, but any work being done to the piece, has to be done by editing the Base Feature that owns it.

Convention would be to build with a timeline, for parametric functions.  Sketches (none) can be edited, and bodies modified.  The Press Pull operations in the first video have not been done in this model.

The red lines are to show if the inside or outside is the cut you want to cut.  All the material above the external outline needs removing - for expected fit.  My understanding is that these bevel / coping cuts, stop the flat pattern, but that latest video didn't seem to care.

As you get going, each of your pipes must be a Component to get each Flat Pattern, to operate as expected.

If you have a version of the file with it's timeline, then use that and abandon this one.

Might help...

[aeronerd]

Thank you again for your help.

I have just quickly made a test shape with a few pipes and cut 2 pipes how i have done the other project. 

Using the method i have done to cope the tubes is there a work around to make the paper templates.

[davebYYPCU]

I could not get anything reliable from your file as downloaded.

I went back and made my split cut as I would normally do it, the Flat pattern goes red, but the inside and outside sketches are working ok, (Sketch on front and back face.)  You decide which one will work for you.

Might help...

[aeronerd]

The problem with cutting a body how you did, is the pipe goes to nothing and that is no good for welding. I need to keep the cope the same thickness all the way around.

[davebYYPCU]

Use the inside sketch.  Removes the bevel edges.

Thats why the Press Pull, is done, and a square cut edge to the surface is the normal process.

Might help...

[aeronerd]

Thank you for trying to help me.

Do you think Fusion might have change a setting in an upgrade and that is causing the issue as to why it isn't woking now?

If i do it how you are saying i am producing a template on the inside of the pipe and i need to be able to place it on the outside of the pipe. 

[davebYYPCU]

Because it is a flat pattern of the same tube, the inside and outside are the same circumference, and the bending allowance is taken up.

It works with a red icon, I think that is cause d by the beveled edges at the coping cuts.  As long as you save the flat pattern sketch as a dxf you will get the paper template cut out ok.

Might help….

[aeronerd]

Probably a dumb question but how can the circumference be the same if the wall thickness is 1in for example?

I have coped approx 200 joints already so it is going to be a lot of work to go back and split with a body not a face. I am also a bit concerned it isn't going to be as accurate as i have multiply tubes all intercepting.

[davebYYPCU]

To be absolutely technically correct, the inside and outside faces are both wrong, the flat pattern is correct width for the k factor position, usually at 0.44 of the thickness.  One inch tube, is a 3 inch plus template width.  

So the inside face should be slightly smaller than the paper cut template, taking up the slot you need for Fusions Flat Pattern.

If doing lots of these, you can set up a Component, with the ready made sketch.   PasteNew, joint to the skeleton sketch.  Alternate workflow to the split body, routine.  Extrude two directions to Object/s.

Might help…..

[TrippyLighting]

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@davebYYPCU wrote:

To be absolutely technically correct, the inside and outside faces are both wrong, the flat pattern is correct width for the k factor position, usually at 0.44 of the thickness.  One inch tube, is a 3 inch plus template width.  

To create a paper template the K-factor should be "1".

f you measure the length edge length of the coped tube, when flattened, both, the inside edge and the outside edge should have the same length.

Setting the K-factor to 1 will make sure the outer edge will remain true and the inner edge is stretched. Or, in other words the neutral fiber - the place of zero stretch - coincides with the outer tube surface.

[HughesTooling · Accepted solution]

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@davebYYPCU wrote:

I could not get anything reliable from your file as downloaded.

I went back and made my split cut as I would normally do it, the Flat pattern goes red, but the inside and outside sketches are working ok, (Sketch on front and back face.)  You decide which one will work for you.

Might help...

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I don't know if this problem with the flat pattern and the example above this one has been answered in any of the later posts but the problem is the split in the pipe is parallel not perpendicular to the tube.

If you construct a triangle and extrude cut through the tube it will flat pattern. I used 1mm to make it easy to see but can be reduced. This works for the example in this post and the one above. Note, if you modify an existing design you need to delete any existing flat patterns and create new ones.

Both versions attached.

[aeronerd]

Thank you so much for your help. You are a life saver. I have been spending so many hours trying to figure this out. 

I totally get it now. Not sure why that example video worked. Your way is probably quicker anyway.

Thank you again for both of your help. Much appreciated.

[HughesTooling]

Didn't watch the video before so thought I'd play around with you example a bit more. I found I can get it to work but it's not very reliable. It seems to depend on which edge you use to create the ruled surface. With some tests using each edge I eventually found one that worked!

What I see now is the surface you created was not planar, if you right click on it you can not create a plane or sketch.

With the edge I found that works it is a planar surface and unfolds but does have the red error in the flat pattern. Like in the video as well.

File attached.