How can I bring a sketch onto a surface?

[autodeskN884Q]

This is basically a follow up to my previous question Solved: My surface offset creates 2 bodies and does not close - Autodesk Community

I want to create an object for 3d printing made out of 2 parts (Bucks, Drips). It's basically a clone of the famous Drippy Bucket in a somehwat different shape. 

 I sketched a triangle with round edges, extruded that, shelled it, measured the loop length of the surface and created a sketch on an offset plane with a width of the loop length. Then I added a couple of "drips" and now I want to bring that onto my triangle

My triangle

My sketch (the width is copied from the loop length field above, not just typed in)

When I now use the Split Face command the sketch loses it's dimensions. Here two examples

When I keep going that solution works fine - but the shape of the drips is wrong as I said.

When I use the Emboss command the sketch keeps it dimensions but there is an artifact left which I can't get rid of

The issue with this approach is that it will fail with offsets later on because of that artifcat. For a more detailed description you can check the previous question which I linked above

[jeff_strater · Accepted solution]

that artifact is from the fact that Emboss uses some approximations, and may not line up 100% at the edges.  The good thing is that you can just delete the artifact:

[TrippyLighting]

When you use the inspect/measure tool, set the precision to "All Decimals".

3 digits are simply not enough. That s why you get that artifact.

[autodeskN884Q]

update: I was in the wrong workspace. Thank you, that worked!

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First of all: thanks for your reply.

But:  Why... does that work for you. 

I tried that before and this happens to me

Before delete

After delete

[autodeskN884Q]

Interesting. Never saw that feature before. Sounds about right but unfortunately the sketch is too wide then / I can't emboss it. Even when I make the sketch slightly smaller 

[HughesTooling]

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@autodeskN884Q wrote:

Interesting. Never saw that feature before. Sounds about right but unfortunately the sketch is too wide then / I can't emboss it. Even when I make the sketch slightly smaller 

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That's a big problem with this tool. Would be quite useful for round objects where it's easy to calculate the circumference but but the command fails if the ends join or overlap! @jeff_strater workaround should work, make sure you're in the solid workspace and maybe window selec to make sure you have all the surfaces of the sliver selected.

Window select from the top like this in the solid workspace then delete.

Mark

[TrippyLighting]

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@autodeskN884Q wrote:

Interesting. Never saw that feature before. Sounds about right but unfortunately the sketch is too wide then / I can't emboss it. Even when I make the sketch slightly smaller 

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In that case, you are doing something wrong!

I almost never post solutions I've not tried before. I did try this successfully before I posted!

This isn't the Fusion 360 Facebook group where you get 100 responses from folks that have all sorts of ideas about what might have worked but never tried 😉

[HughesTooling]

@TrippyLighting  How did you measure the length? I used measure set to all, measured one edge and one arc then had to use a calculator to come up with 500.3452827705975 mm

And I get this error.

[HughesTooling]

@jeff_strater Thought I'd try calculating the length using a reference dimension. Seems to work in the parameter manager but fails to solve in the sketch and shows the wrong size. Don't think I'm doing anything wrong as the calculation and reference are in the same sketch, any ideas why it fails. File's attached.

[TrippyLighting]

Ahh, I see! 

I selected the bottom face. That provided me with the loop length.

Then clicking on the measured value copies it into the clipboard :

I had actually created a screencast at least 30 minutes ago and it still hasn't posted 😕

[HughesTooling]

@TrippyLighting Thanks, can believe I didn't think of that!🙄

Part of the reason I didn't think this would work is every time I've tried this on a simple cylinder it fails. Just tried again and it fails using PI*diameter or the measured length, see attached file.

Also having to measure, copy then paste does mean the model's no longer parametric. Using a calculated size fails even though it's a simple enough calculation. 3*face length from a driven dimension + PI*(2*corner rad). The measured size and calculated are different, guess the parameters are rounded.

The driven dimension is only showing 5 places so might be the problem, don't know if there's a setting for this. Really could do with a tolerance allowance in emboss. File for the part from this thread also attached with calculated length.

Thanks Mark