component to sheet metal

[Anonymous]

these are the components i want to convert to sheet metal how do go about doing this ?/?

[laughingcreek · Accepted solution]

converting this to a sheetmetal part would take a lot more work than just using the sheetmetal tools to make it right from the beginning.  but before you do that, I would suggest going back through the tutorials and getting a handle on parametric solid modeling.  and why did you delete your sketches?

[chrisplyler]

There is no "convert" function.

You can turn a body into a sheet metal body by creating at least one sheet metal flange, then combining a regular body with it. But the regular body has to have been modeled in a way that will allow it to become a sheet metal body. It will have to be modeled to match the sheet metal rules.

You're model has hard corners. A sheet metal body has BENDS. I've made a video for you. It's looking head on at the edge. The first half shows one of your components...then it shows a similar sheet metal body in the same place. See the difference?

https://knowledge.autodesk.com/community/screencast/c9e8ede3-c485-477d-b583-2b8be062e9c4

[TheCADWhisperer · Accepted solution]

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@chrisplyler wrote:

There is no "convert" function.

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Actually there is, assuming the geometry was created correctly.

This was new functionality  added in a recent release.

[chrisplyler]

Oh wow! Hadn't discovered that.

[nathandiclaudio]

I have a part that I modeled in another app, then imported into Fusion to try and convert it to sheet metal.

The part has a bend in it.  I can pick a face to allow Fusion to create rules, but the bend is ignored when trying to unfold or flat pattern.

The part is basically a .125" thick plate with a ~20 degree bend.  Fusion detects the thickness of the body and creates a rule based on that.

I am able to add flanges to the part once converted to sheet metal, but that's it.

Is there something I'm missing?  Will Fusion only correctly covert flat solid bodies to sheet metal? 

Thanks.

-Nathan

[Warmingup1953]

I'm no expert but does the Body comply fully with sheet metal rules? Seems like a simple question but in my experience, there can be violations of the rules in unsuspecting ways especially in regard to thickness and bend radii.

[laughingcreek]

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@nathandiclaudio wrote:

...Is there something I'm missing?  Will Fusion only correctly covert flat solid bodies to sheet metal? 

Yes, you're probably missing something.  if modeled correctly you can convert a solid with bends to Sheet Metal. to get help with that you can post your model (export as a .f3d file and attach).

[TheCADWhisperer]

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@nathandiclaudio wrote:

I have a part that I modeled in another app...

The part is basically a .125" thick 

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Attach the original file here.

It either is or it isn't .125" thick.  If it isn't uniform thickness then it won't unfold.

[nathandiclaudio]

F3D is attached.

It is .125" thick.  

I also checked that the bend radii modeled matches the rules as far as I can tell.

I'm new to Fusion, and I appreciate the help.

Thanks

[TheCADWhisperer]

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@nathandiclaudio wrote:

I have a part that I modeled in another app...

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Can you Attach the original file from other app?

The cut edge is not perpendicular to the flat in this area...

https://www.youtube.com/playlist?list=PLp5izJt_zvN29W2cEFHAK949eImc9xFOT

[nathandiclaudio]

Good catch, I just checked and the original STEP is that way.
That is my mistake. It was created because of how I went about modeling it and didn't notice.
I was too wrapped up in thinking the radii was the issue to see it.

I'll repair that and try again.

On a side note with radii, if the inside bend radius is .063" per the rule, but I create a .0625" radius in the model, I'm wondering if Fusion will cooperate in the conversion.

Full disclosure, I'm using Shapr3D to model these parts and then convert them to sheet metal in Fusion.

Thanks!

[laughingcreek]

the thickness on either side of the bend line is off when you check past 3 decimals.  here's a way to correct for that-

[TheCADWhisperer]

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@nathandiclaudio wrote:

Full disclosure, I'm using Shapr3D to model these parts and then convert them to sheet metal in Fusion.

For something this simple - time to start learning how to model in Fusion 360 rather than attempting to convert.

[laughingcreek]

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@nathandiclaudio wrote:

...if the inside bend radius is .063" per the rule, but I create a .0625" radius in the model, I'm wondering if Fusion will cooperate in the conversion....

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The radius doesn't have to match the rule (nor does the thickness) to properly convert.  but the relative size of the radius on the inside of the bend to the radius on the outside of the bend do have to be correct.  those weren't right in your model either.

outside radius = inside radius + material thickness

[nathandiclaudio]

Yes, true. I do have an understanding of how to create sheet metal parts in Fusion, but I need to do it more.

The conversion reasoning for me is mobility. I don't have a laptop, and I'm not in front of the computer often.
I was hoping that the addition of "convert to sheetmetal" would allow me to design parts away from home using an app like Shapr. Not ideal, I know.

Thanks.

[nathandiclaudio]

Thanks, I thought inside radius was .5 of outside radius.
I have a lot to learn. Ha