Convert To Sheetmetal - Thickness Error Message

[salesYEXHJ]

Hi Everyone

We are trying to convert a drawing into a sheetmetal format so that it can be laser cut and CNC bent for us.  We have watched and are following the example provided in the 360 Live Tutorial: Creating HVAC parts in Fusion 360 Sheet Metal https://www.youtube.com/watch?v=oGwn6SsyPwA

While we were able to get it to work in the tutorial example we can't get the procedure to apply to our own design.  I am not sure what we have done differently.

Screencast link https://autode.sk/2AVnbrY

Thanks in advance for taking a look at this for us.

[TheCADWhisperer]

File>Export and then Attach the *.f3d file here.

Your Loft surfaces are twisted - they are not planar.

Be careful where you are getting your sources of information.

[salesYEXHJ]

File Attached to my reply post.

To untwist I'm imagining using a polygon with more sides?

[TheCADWhisperer]

Your sketches are not fully defined.

Your problem does not match the video that you linked (twisted surfaces).

Indicate timestep of video that you are relying on to indicate that this is possible in Fusion 360.

[TheCADWhisperer]

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@salesYEXHJ wrote:

To untwist I'm imagining using a polygon with more sides?

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Can you make a decision on exactly what you want (your lines in Sketch1 are not all 4 inches).

Do you have a similar existing part in the real world?

[TheCADWhisperer]

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@salesYEXHJ wrote:

To untwist I'm imagining using a polygon with more sides?

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Is something like the Attached what you are after?

[jhackney1972]

I used your measurements as much as possible but as @TheCADWhisperer said, your sides were twisted since you were coming from a octagon to a hexagon.  I change the small sketch to a octagon to match.  You also will have to add a fillet to the seams of the stitched surface, I used .188 radius, in order to make the conversion and flat pattern to work.  Model is attached.

[salesYEXHJ]

I'm getting closer thanks to both of you

The twist problem made sense as soon as it was mentioned.  

Not being fully defined was something I hadn't noticed but have been able to fix

At which stage does one add the fillets?

Order....

sketch1

sketch2

loft 5 sides

stitch 5 sides together

add thickness

fillet 4 bends

convert to sheetmetal

I seem to end up with individual sections and not a single piece of sheetmetal

file attached of my revised work including fully defined (and slightly modified) sketches

[jhackney1972 · Accepted solution]

You would add the fillets after the individual lofted surfaces are fully stitched together.  I will not be available too look at your model for a few hours as i am away from my computer.  You have to make sure you have successfully stitched ass individual lofted surfaces together before moving on.  After stitching you should have one surface body.

[JDMather]

You still have two twisted faces.

If you can't create a sketch on the face - then it is not planar.

(Also, this can be done with one Loft (didn't you look at the file that I attached earlier) and the fillets are done before Thicken (again - this was demonstrated in the file that I attached earlier)).

[TheCADWhisperer]

Here is another example using your latest attempt (see Attached).

[salesYEXHJ]

Thanks again CadWhisperer

After you mention it I again can see the twists and it makes sense that that is the problem.  That makes it seem like a dimension issue between sketch 1 and sketch 2 I think?

I notice that it looks like you needed a change to the face lengths on some of the smaller octagon (sketch2)?  That is no problem for the real world us of the part....I'm having some trouble following the thought process on how you decided those lengths though.  It appears to be the solution that I was missing though

I would like to understand so I can apply the knowledge in the future if possible

[TheCADWhisperer · Accepted solution]

The key is that the lines have to be parallel from one sketch to another in order to create planar faces.

(BTW, this isn't a limitation in Autodesk Inventor Professional where you can create Lofted Flange sheet metal parts directly.  Students can download Inventor for free.)

[salesYEXHJ]

Thanks again for the help guys.  Progress has been made now for sure

When adjusting the smaller octagon was there a formula or strategy used?  Or just some trial and error until the faces straightened out?

[TheCADWhisperer]

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@salesYEXHJ wrote:

  Or just some trial and error until the faces straightened out?

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No trial and error.

I simply changed your octagon to construction - you could make it ANY size you want.

The key was making Lines 1 and 2 the same length as your lines.

After that - everything was driven by the size of the octagon.

Because all lines must be parallel - there was only one possible solution for the remaining 3 lines.

Now, if you didn't place Line 3 on the octagon - there are other possible solutions (longer to the left, shorter to the right in image below).