3D Sketch to Flat Pattern.

[TinWhisperer]

I am looking for advise or work flow to go from a 3d sketch to a flat pattern .

I am going to use 26 ga galvanized material so it about .021 in thickness.

I have read through a few post on this site and checked out the couple available you tube videos but i find it does do not give me  the flat pattern  sometimes , most of the time.

I am trying to come up with flow so I can build any crazy transition in 3d sketch and make it flat.

I have and still use sketch up 8 pro with the "flattery" add on which work decently and will convert just faces to a flat pattern. 

but, I trying to covert all my work flow to stay within the fusion 360 ecosystem.

is there a way do convert surfaces / face to a flat pattern in fusion without thickening the face to a body? as if I was using a material like paper?

thank you

[TinWhisperer]

For sure my original drawing I presented was done in my old methodology with just faces so unlike something in the real world it doesn't have any thickness.

Fusion cannot simply unwrap surfaces or faces, apparently and they need to have thickness so it can mimic what's happening in the real world.

So the only way to use fusion is to have a body or a sheet metal body not just a surface to create flat patterns.

Metal in the real world deforms on its bend lines. fusion 360 adds this deformation into the pattern to improve its accuracy.

I do get these points you're trying to make.

I also am pretty sure in the math background of fusion 360 it's using triangulation to figure out those flat patterns and then adding in the k Factor or thickness of whatever other sheet metal rules you've added. Even though it visually represents it to you as an ark it could not make a flat pattern that arc information ,deep down it's a whole bunch of facets.

Weather fusions allowing you to see that hidden geometry or not.

I've also had this conversation a few times over the years. What I can tell you is I have actually made and installed hundreds of square to rounds in the real world. 

And I'm here trying to figure out better more accurate methodology.

[TinWhisperer]

Are you in agreement with me that the images in Message 1 & 3 are incorrect simplifications?

I will meet at "simplified" 

I need to establish that the simplified example you presented does not accurately represent the real world

I agree that the fusion360 model is more accurate in representing the real world. 

I have had this debate many times over the past 20+ years.

There is definably a few schools of thought and points of view on the subject.

[TinWhisperer]

Run through this work flow a few more times and it turns out the you don't radius corner to your sketch.

Once you convert to sheetmetal and unfold fusion360 takes care of adding to the corner according to material rules.

I do not have a faceted round on this one . trying that next. 

[TinWhisperer]

Tried 

Rectangle with radius corners to 12side polygon:

fail to create flat. Likely breaking rule #2 in sheet metal if i am starting to catch on .?

Rectangle with square corners to 24side polygon:

fail to create flat. Likely breaking rule #2 in sheet metal again?

Rectangle with square corners to 12side polygon:

fail to create flat. Likely breaking rule #2 in sheet metal again?

Rectangle with square corners to round:

Created a flat pattern in Message 23 . Conical corner even to a point still passes rule #2 in sheet metal ?

Rectangle with radius corners to 12side polygon:

Created a flat pattern in Message 2

Things are starting to becoming clear as far as workflow.

still filling in the blanks.

[TinWhisperer]

This is the cleanest flow yet only 9 surfaces . Seem like will only do square corner at the bottom with circle at the top (rule #2 passed?) 

Still would like to work out so simple flow for polygon to polygon without breaking rule 2

. I am missing a puzzle piece ( step) here

[TheCADWhisperer]

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@TinWhisperer wrote:

I also am pretty sure in the math background of fusion 360 it's using triangulation to figure out ... ...deep down it's a whole bunch of facets.

What I can tell you is I have actually made and installed hundreds of square to rounds in the real world.

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I don't know the algorithms in the background, but I suspect that Fusion only uses Facets for display/shading.

I think it uses more sophisticated math for the spline curves on the edge of this Flat Pattern.

I don't see a sharp corner in the image of the example that you attached.

I think when we get to the shop floor - we do what works.

There shouldn't be any "schools of thought" as this is geometry.  It is what it is.  It is not a sharp corner.

I am confused whether you want a polygon end or a round end?

Your image of a real part and your *.f3d file increasing sides of polygon leads me to believe that you want a circular end and are attempting to approximate with short straight lines.  If so, why not use a circle?  See Attached.  (Click on Flat Pattern.

You can have as many bend lines as you like.

[TinWhisperer]

I am confused whether you want a polygon end or a round end?

Originally I was fix aided on having a 12 or 24 polygon on top but my mind has rapidly begun to change.

Ideally now experiencing what can be done with f360 I would like a methods for :

Square to Round - which you solved in message #2 - thank you

Polygon to polygon - which I am still foggy on the on the bend lines, filet, radii, workflow.

I don't see a sharp corner in the image of the example that you attached.

I cant argue that.  no truly sharp corners in reality. Zoom in on the facet of a diamond enough it would be rounded over.  

In the future maybe a method when the planes are not parallels weather polygon or round.

( so I could have a square to round or polygon to polygon or round to polygon at a 45 deg or 70 deg or whichever I chose) 

I think it uses more sophisticated math for the spline curves on the edge of this Flat Pattern

I agree on that for the curve of the edge but I still believe the true points it follows are triangulated.

Either way it is magic what Fusion 360 can do.

You can have as many bend lines as you like. 

Yes, definitely would like more or less of these depending on how big the fitting is. 

[TheCADWhisperer]

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@TinWhisperer wrote:

You can have as many bend lines as you like. 

Yes, definitely would like more or less of these depending on how big the fitting is. 

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Did you see how I had to manually add the bend lines in my latest attachment.

I think I had it automatically use the Loft Rails in the past to generate intermediate Bend Lines in the Flat Pattern, but now have to add manually.

Divide up as many times as needed.

Also - I made a mistake in my original reply with the location of the 4" offset, but that is was easy to edit in my latest example.

[TinWhisperer]

• Thank you for the file when I get back to my computer tonight I'll definitely look through it thoroughly.

[TinWhisperer]

Thank again you the file.

I ran through it a few times.

Step 8 you used this trim surface tool.

what a great way to go about it. 

I was creating a sketch and then extruding it to make the cut out.

what are the advantages of using the trim surface tool?

Step 10 you used the flange tool on Sketch 3 to create sheet metal body 2.

this is how we convert it instead of the convert to sheet metal tool?

how are sketch 5 and body 1 connected I feel like I missed something here.

I'll continue to review the file , I define have a  few holes in my fusion knowledge. 

Your idea of manually drawing in bend lines on top of the flat pattern makes senses.

I see you divided the panels by degrees (42.1/3)*1deg

( I also like writing formulas in the dimension boxes and use fractions for infinite remainders) Both great tips

I took a different approach on how to divide up the bend lines.

I used "points along path" to divide the top curve even by length so ultimately it would divide the circle evenly. (in this case by 12)

I did find "points along path " tool slow to do this one point at a time. Is there any other methods for dividing a curve evenly base on length in Fusion 360? 

I will continue to review this most recent file.

I am pretty excited to implement this shop soon.

[TheCADWhisperer]

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@TinWhisperer wrote:

Step 8 you used this trim surface tool.

what a great way to go about it. 

I was creating a sketch and then extruding it to make the cut out.

1. what are the advantages of using the trim surface tool?

2. Step 10 you used the flange tool on Sketch 3 to create sheet metal body 2.

this is how we convert it instead of the convert to sheet metal tool?

3. how are sketch 5 and body 1 connected I feel like I missed something here.

4. Your idea of manually drawing in bend lines on top of the flat pattern makes senses.

5. I took a different approach on how to divide up the bend lines.

I used "points along path" to divide the top curve even by length so ultimately it would divide the circle evenly. (in this case by 12)

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1. Using Trim Surface ensures that when Thicken is used the cut edges are perpendicular to the flat face in Flat Pattern - especially important if the cut crosses a bend or angle.  Otherwise could end up with double lines in dxf for edge.

2.  Convert was not originally in the Fusion Sheet Metal tools - I guess I am stuck on the old way.  Either way works on this one.

3. See #2.  Not really needed if just using Thicken and Convert to Sheet Metal.  But for the sketch I selected P for Project and selected the surface "face" to project the boundaries of the "face".  (Face is actually term for Solid Bodies - this was a boundary of part of the surface.)

4. As I think you noted in Brad's video - I think at one time Fusion would create from the Loft rails (guide curves).

5. Excellent!  That is what I originally intended to demonstrate - but I had trouble a gave up too quickly.  Bravo on this technique (when it works).  As far as dividing - I am used to using Reference (driven) dimensions in equations in other CAD softwares, but unfortunately Fusion does not permit that at this time.  A lot of the parts that I do >> cannot be done in Fusion << yet.  

[TinWhisperer]

Brought one into reality today.

it fit very nice.

I added allowances to the pattern for the collar edge, lap seam and slip and drive connection.

The first ever CNC cut square to round  I have made.  I 've hand cut and made very many by hand.

Thank you @TheCADWhisperer I' am going to keep reviewing this work flow and see how it can be done in the fewest steps possible and the most universal for different shape types.

A cut video and DXF attached. 

Tomorrow I'll pull out some different rollers put a more proper bead on the collar of the next one.

Very happy so far

[TheCADWhisperer]

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@TinWhisperer wrote:

Thank you @TheCADWhisperer I' am going to keep reviewing this work flow and see how it can be done in the fewest steps possible and the most universal for different shape types.

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It sure is fun to see a design taken into the real world.

And it is a pleasure to work with someone with an aptitude for observation and discovery.

The standard sheet metal modeling techniques are easy enough to figure out, but if you haven't seen these two videos - they demonstrate a hybrid technique that you will likely need at some point.

https://www.youtube.com/watch?v=BAa6J0Pigp0&list=PLp5izJt_zvN29W2cEFHAK949eImc9xFOT&index=1

https://www.youtube.com/watch?v=j4Agn8bWKZY&list=PLp5izJt_zvN29W2cEFHAK949eImc9xFOT&index=3

[TinWhisperer]

I really enjoyed the experience too.

I plan on adding to this thread as progression happens. I could ( accept solution ) but I am not sure which message I would select,?#2 lol . I do believe a cleaner flow is yet to come, I plan on sandboxing this for a while.

Currently its down to 15steps (if you count SAVE file at the beginning and export DXF at the end)

Ultimately to have a clean F3D file where we can simple input ; height , diameter, rectangle size and offsets both y and x, bend guide spacing  and hopeful one day non parallel planes.  

I did change 13inches  to 18inches  in the rectangle on last F3D you sent and it did update the model from the sketch right to the flat pattern perfectly.

you can see I nested and cut two 13x3.5 and one 18x3.5 in this picture.

Thank you for those video links, I will comb through them.

This has sparked my interest in the fusion360 Sheetmetal environment. I plan on learning as much as possible about this space.

very excited about of the path(s) to reality to come.