Fusion 360 crashes when i try to edit sketches.

[justo_urbina12]

Hello guys, since the last update Fusion 360 crashes when i try to edit sketches. Any suggestions, thanks for reading.

[jeff_strater]

It looks to me like your sketch is very complex - I see a large number of mirror/symmetry constraints.  I wonder if the solve is just taking a while.  How long have you left it running before killing it?

Were you able to do things like add your tangent constraint before the update?  It could be that some performance change in sketch was introduced in the update, but we haven't heard of others seeing problems.

And, if it would be possible to share your design, we can take a closer look and see if it is really crashing or just slow.

thanks,

Jeff

[justo_urbina12]

Thanks for replying, how do you want me to share my design?

[jeff_strater]

I always just use the "share public link' command to share designs, from the data panel on the left;

This brings up the following dialog, make sure the two checkboxes below in blue are checked:

Then, copy the link and either post it here, or use a private message to send it to me.

Just FYI:  I will be out of the office next week.  I will pass this off to someone if I am not able to get to it myself.

Jeff

[justo_urbina12]

Here it is http://a360.co/1WMieUI, thanks Jef for your help.

[innovatenate]

Hi there!

As soon as I opened the design "Sketch2" & shield "sketch" had lost reference to the base plane. To correct this, I can right click on the sketch in the timeline and select Redefine Base Plane. I'm not sure if this is happening in your model or not, but thought is was worth mentioning.

I tried adding the tangent constraint just like you and then Fusion 360 became busy. I waited for a while about an hour, but the operation never finished. I think what Jeff mentioned above is still a good point.

Are you inserting a DXF, DWG or an SVG to create this sketch? If so do you have the original file? This sketch geometry seems like it was imported from somewhere. Is that correct?

If it's a DXF or a DWG, you may be able to edit the file in another application. In the other application, you can add the sketch entities to different layers. This will help to move sketch entities into separate sketches in Fusion 360. The other thing that may help is to delete duplicated geometry.

Also, is it possible to simply delete the mirrored geometry? Deleting the mirrored constraints and mirrored sketch geometry may make solving much faster/easier. There are a lot of relationships created from that operation.

Otherwise, if you can't use the layer trick mentioned above, you may have to copy/cut and paste some sketch entities into separate individual sketches to help reduce the computational overhead. The fewer sketch entities per sketch, the faster it will be at computing a change like adding a tangent constraint. 

I hope this information is helpful. Please let us know if you have any questions.

Thanks,

[jeff_strater]

Thanks for the model, @justo_urbina12,

I took a quick look, and tried adding that tangent.  I let it run for quite a while, and it never finished.  I suspect, though, that if you let it go long enough, it would eventually finish.  But, that's not practical.

So, I will have the sketch team take a look, but I suspect that they will just say that there are a lot of symmetry constraints in this sketch.

I have a question for you, though:  In this sketch there seem to be two copies of the main sketch geometry:

What is your intention with these two copies?  I believe that this is what is making everything so slow.  If you intend to use the mirror for making a solid body, I would strongly recommend you use the Mirror Feature to do this rather than try to use sketch mirror.  The performance of Mirror Feature will be significantly higher than with sketch mirror.  In fact, you should be able to get very good performance using this method, both in your original sketch and in making the mirror.

So, give that a try:  delete the mirrored copy of the geometry (even this takes a couple of minutes).  I tried this, and then I was able to add that tangent constraint without a problem.

Jeff

[innovatenate]

Below is a quick video showing how quick that tangent constraint is after you delete the mirrored sketch entities.

Attached is a sample DXF file that has been layered in AutoCAD and the resulting Fusion 360 design. I hope you'll find the performance is much better.

Thanks,

[justo_urbina12]

I just opened up the layered design in Autocad, my question is when i run into this problem should i layer a sketch all the time? Thanks your help.

[justo_urbina12]

Yes this file is an svg.

[justo_urbina12]

The reason why i mirrored it is because i couldn't edit the lines on my fist sketch without Fusion crashing, so i tried to delete the first sketch but no luck.

[justo_urbina12]

Ok i uploaded the layered sketch in Fusion an i was able to tangent arcs, however i am unable to extrude the way i want it to be extruded just like the design.

[innovatenate]

Can you extrude in oppisite directions to achieve the desired effect? If not, you can extrude as a new solid body. After creating multiple solid bodies, you can use the move or the align command to reposition those bodies. When you're satisified with the position, go ahead and use the Combine command to merge the bodies together. 

Does that help?

Thanks,

[fulcrumusa · Accepted solution]

I think the reason why you can't extrude inner parts of the sketch is because you are using press/pull. By default, press/pull will try to use the body under which the cursor is located. You can try one of the following:

1. Hide the body before attempting to extrude the inner parts of the sketch, or

2. Hold down the mouse button when attempting to select the sketch. This should popup a menu allowing you to select which feature to press/pull, or

3. Use Extrude rather than Press/Pull. That command defaults to sketch geometry rather than bodies.

I hope I understood your problem correctly.

[justo_urbina12]

As soon as i get home i am gonna try what you've suggested, thanks.

[justo_urbina12 · Accepted solution]

Yes indeed you understood my problem, here is Link's shield is ready to be toopathed and machined, thank you so much for your help.

[crh5055]

I am having a similar problem.  I am new to Fusion 360, so I am probably doing something wrong.  With the linked file, I try to add a circle (anywhere, any dimension) and the program crashes.  What might I be doing wrong?

http://a360.co/2icKlhG

[jeff_strater]

Hi @crh5055,

Can you post a screencast of the crash?  Do you get a crash report dialog?  If so, did you submit it?  I tried just adding a circle to this sketch, and it seemed to work OK for me:

Thanks for any additional information you can provide to help us figure this out.

Jeff

[crh5055]

[image: Inline image 1]

Here's what I get when I add a circle from the origin with diameter 7.25".
It draws the circle, then crashes without a dialog. I added the diagnostic
log file to this message, if that helps. I am new to this tool and am
trying to learn how to use it. I have had some success designing other
gears, some of them more complex than this one. Another clue is that I
inserted the gear outlines, including the involute shape by inserting an
SVG file.

I really appreciate your help.