Problem with creating sheet metal flanges on straight edge adjacent to a curve

[antswanmail]

Dear gurus,

Is it possible to create a sheet metal flange on a curved edge? You can see in my file attached that I have a vertical flat surface which then runs into a curve. I want to create a flange along the bottom edge of the flat surface, which you can see I have done (the part with the holes in it). The only way I could achieve this was to split the component into 2 bodies, probably because the program didn't like the curve which is joined to the straight section. Now I am unable to create a flat pattern of the whole component. Is there a better way to do this?

Also, I would like to create another flange at the end of the curved section furthest from the straight part, to turn the vertical edge in slightly. The program will not let me do this, I'm guessing because of the curve. Is there any way to achieve this?

Thanks, Anthony

[davebYYPCU]

I was able to Flat Pattern your body 1, then deleted that, see below.

I was also able to hide Body 3, and make Body 4, as a one piece body, that also Flat Patterns.

Whilst I don't have the expertise to remake the two bodies into one, by adding the bolt hole section to Body 4, but know that it can be done.  So with the parts as you have them should be able to be one piece that does Flat Pattern.

I didn't know what you wanted to do at the other end of the body 4.

The main thing you may have missed is that you can only have one Flat Pattern per Component, so your model needs all flanges to be added to make one body as the file exists at the moment.

Might help....

[chrisplyler]

Screencast will be displayed here after you click Post.

e84c2a77-6c4e-486b-8741-ee952d2d7f5c

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@antswanmail wrote:

Also, I would like to create another flange at the end of the curved section furthest from the straight part, to turn the vertical edge in slightly. The program will not let me do this, I'm guessing because of the curve. Is there any way to achieve this?

Thanks, Anthony

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Not with Sheet Metal, no. Bends must be conical or cylindrical. That's the only type of deformity that Fusion can handle. The stretching/compressing of metal that happens when you put a bent edge through some type of edge roller, or hammer it over the edge of a table or whatever, is not supported in Fusion.

If you want it functional, you can add some extra width at the curved portion, and then in real life you can roll it over or whatever, but it won't be shown that way in the model. If you want it to look right in the model, you can sweep your desired shape along that curved edge while in the Model workspace as a separate Component so that it looks right, but it isn't going to be part of the Sheet Metal Component or show up in its Flat Pattern.

[antswanmail]

Yeah, I guess maybe there is no way to create a flat pattern of the whole object at once.

[davebYYPCU]

Well there is nothing so far to make me think that.

Nobody knows about the additional missing bit,

that it has to be Sheetmetal compatable, and you

need the whole body as one piece to facilitate a Flat Pattern.  

Certainly the 2 flanges in the file so far can be made to Flat Pattern.

Add the missing bit (to turn it in a bit) to the file, so the mystery can be cleared up.

[antswanmail]

OK, see the updated file attached. This is the part I am trying to make but I would like to be able to flatten it out completely. You can see in the picture below that when I turn it into a flat pattern it does not flatten completely (the arrows are pointing to the remaining curves).

Thanks

[davebYYPCU]

Well a bit closer, Your sketches are not accurate enough (or fully defined,) for Fusion,

The faces of body 1 is not colinear with Body3, there is a step.

and I don't know sheet metal well enough to fix it, but

Your body 1 and 3 should be a one piece extrusion 1 inch high, (Will Flat Pattern as per previous pic)

with the bolt plate and the end curve flanges added to that single body (joined) 

To Flat Pattern, build one body, by adding the Flanges to it,  just like you did for Body 1

You have combine joined body 1 with 3, 4, and due to the sketch misalignment, will not Flat Pattern.

Might help....

[TheCADWhisperer]

This is an easy problem - but none of your first 3 sketches are not fully defined?

Have you gone through the Tutorials?

[davebYYPCU]

I got the majority of it working so far, all but the last flange, wont select the body edge.

Will be lurking....

[TheCADWhisperer]

See Attached.

I crashed Fusion a couple of times and didn't get Offset on Flange to work - so I had to use hybrid technique.

Have to go to work in a few minutes so no time to go back and look at Offset issue.

[chrisplyler]

You can't flange off of a bend. You'll need at least a tiny straight bit at the end of that large radius bend in order to flange off of. That's why, in the above Screencast, I add a .01-inch straight line to your sketch include it in the first flange upwards.

[davebYYPCU · Accepted solution]

Yeah, that’s where I was stuck, but that short extension was in the original file, from @antswanmail , but I had not caught on to why.  Thanks for that.

if it were mine, I would add the last flange to the first sketch.

@TheCADWhisperer  Not reviewed your version yet.

[chrisplyler]

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@davebYYPCU wrote:

if it were mine, I would add the last flange to the first sketch.

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If you wanted it to match the Rules in place, you'd have to match the outside radius of the new one to that other one. Other than that small detail, I think your suggestion would be no problem.

[davebYYPCU]

Honest I had not reviewed the file, at that time, I see you did what I was thinking, nice.

[antswanmail]

Thanks everyone for your help, I got it to work.

I re-drew the sketch with the last flange in the first sketch (I did not know the program would treat that as a flange - good to know). I also encountered the problem of the offset flange for the part with the holes in it causing the program to crash. I solved this by making the edge slightly shorter and doing a full edge flange instead and then extruding the offset part. I was then able to get a complete flat pattern.