can't extrude projected outline

[calexpavel]

I want to extrude the outline of my projection in order to cut from another body. It only partially extrudes the curves. They should be planar, since i projected it on a flat surface. 

I tried to do it with a cilinder and it works, so i guess it's the shape i want to extrude too complex, or what?

Any idea why this doesn't work? Thanks!

[JDMather]

Is there a reason that you are working with Capture Design History turned off?

Gap

[calexpavel]

The geometry is imported and history is off by default. Does it have to do
with my problem?

[JDMather]

No, but history makes it easier to diagnose.

When I import geometry the first thing I do is turn on history before moving forward.

There are quite a few gaps in your sketch.

If you go to the Surface tab and attempt to Extrude with Chaining turned on - you can quickly diagnose.

If I had history, I would use the divide and conquer technique.

I think your best bet would be to trace over this since the geometry is so simple (I did not try to go back and diagnose the original source of the issue).

[calexpavel]

I uploaded the file with history. There really isn't much to see in the history. 

When i extrude with chaining, it doesn't select the whole outline.

I try to zoom in where it disconnects to see if there's any line missing but when i zoom too much the geometry disappears. 

I try to find that gap that you found but i can't. Is it so small that i have to zoom more? How can i zoom more without geometry to disappear?

If there's a gap, why is it? 

Thanks for help!

[g-andresen]

Hi, 

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@calexpavel wrote:

1. I try to find that gap that you found but i can't. Is it so small that i have to zoom more? How can i zoom more without geometry to disappear?

2. If there's a gap, why is it? 

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1. I prefer the  "moving a single or crossed line method". (in this case there are several gaps).

2. Sometimes it happens while projecting profiles, don´t kow why.

günther

[jeff_strater · Accepted solution]

"If there's a gap, why is it? "

see this thread for a detailed explanation:  https://forums.autodesk.com/t5/fusion-360-design-validate/intersect-sketch-accuracy-issue/m-p/684944...   See message #5.

The short version is:  When dealing with imported geometry (and a few other cases) the bodies can be somewhat dirty in terms of tolerance.  These gaps are caused by that tolerance in the model.  The only way to fix them today is to bridge the gaps yourself.

[calexpavel]

Oook, i think i know what you're doing. You are drawing a line and if the sketch from the line to one end is closed, there is no gap, but if the sketch is open, it has a gap. And  you can narrow the area down by moving the line. Nice trick! Thanks!

I wish fusion had a command to find the gaps, like rhinoceros3D has "zoomNaked" command to show you gaps in surfaces. Also, it's hard to zoom in and find the gaps, even if you narrow down the area.

[calexpavel]

Thanks Jeff.

It feels so good to know why this happens at least, even if it doesn't solve the problem.