Sketch Mode Significant BUGs? Episode 2, Copy and Paste - Paste ERROR

[OFGLLC]

This is a continuation of why Fusion 360 is not really ready to be adopted for art work, such as one might cut with a 2D cutter such as plasma, laser or water jet.  Episode 1 is far more critical but seems to have stalled in the Autodesk community without any solution.  These are serious problems that can be encountered by anyone using the Sketch mode.

This episode is about pasting a simple sketch content to another sketch in the same design.  This should be one of the simplest things to do but it has a flaw (besides the horrendous Episode 1 ERROR).  It is:

   1)  When the copied sketch content is pasted, it is rotated 180 degrees.

Why is this a problem?

   1) The reference to the location in the grid from the first sketch is lost when you rotate it.  Now you have an issue with re-indexing it to the original sketch if you need to do so.

   2) One you use the manipulator to rotate it back to its correct vertical orientation, there is some kind of orientation recorded in the data.  Then when you export as a DXF file, which you are certainly going to do because Fusion CAM is not anywhere near ready to encode a file to a controller efficiently that has the ability to control a torch height system or control height and feed rates and accelerations for small problem areas. you are gong to find that it is rotated in that CAM system.  Is that an issue with the CAM system, in that it doesn't utilize the orientation that Fusion is clearly recording in the file?  Yes, and that may be corrected, but since all we wanted in the first place was a copy in the same orientation on the screen. it should not be that way in the first place.

(Note:  Fusion CAM is solid oriented.  Great for Milling, I love it.  For 2D, its impractical for more reasons than this post deserves)

So, through this episode 2, the current status of the Sketch mode is that when you copy from a sketch to another sketch, you will likely lose arc lines or have them deposited somewhere randomly with a mess of unmovable points and the paste will likely, but not always, be rotated 180, so that it appears upside down.

Sample Design:   http://a360.co/2ih4ShG

Jeff

http://a360.co/2ih4ShG

[jeff_strater]

I tried to reproduce this in your design.  I edited the sketch "Border Collie", copied the sketch geometry, exited the sketch, then created a new sketch, and created a new sketch on the same plane as that sketch, pasted the geometry, and it seemed to be corrected oriented:

In your design, I'm not sure how Sketch 2 was created.  What plane was used to create it?  Sketch copy/paste will always paste the geometry in the same orientation with respect to the sketch's XY coordinates.  So, Sketch 2 must not be based on the same plane as "Border Collie".  This is expected. 

From the same view, here is "Border Collie"'s coordinate system:

And here is Sketch 2's coordinate system:

 

However, even so, it is very easy to get the geometry into the desired orientation by simply changing the pivot point, and rotating by 180 degrees:

Hope this helps,

Jeff

[OFGLLC]

Every thing is on the same plane. There are no other planes defined in the design. You would see them as a construction in the design if there were. There is no reason for another plane in a 2D project that will be cut out of sheet stock. Sometimes it works. We have this problem maybe 6-7 times a day.

[OFGLLC]

Note that the object in this Sketch is intentionally copied at the maximum resolution that will fit on the screen to avoid Episode 1 ERROR.

[OFGLLC]

Jeff,
A little more information, now that I have a moment.
My daughter and I have tried every conceivable sequence of creating sketches and positioning mouse pointers, using different menus, anything we can think of.  
Sometimes, by closing Fusion we can get a copy to paste when a design is reloaded.  Even that is not consistent.  This is why I did not include this in Episode 1, which is more serious and totally replicatable by following the post.

I’m sorry, but the sequence you saw in the screencast I provided is sometime how it works.  If someone could say, do it this way and it will never happen, we would be thrilled but after trying for nearly a year, we haven’t found it.

(We always select the Z plane, the flat one in the perspective view.  I suspect the view is possibly wrong but I don't know how to tell.  I have never been able to coax the Redefine option to display the plane selector.  One of the things we try to remember is do is to be in perspective view when we create a sketch.  When you are working fast, steps you wouldn't expect to need can be skipped.


this Jeff

[jeff_strater · Accepted solution]

Ah, I see what's happening.  I had to watch your screencast 3 times in very slow motion to see it.  Here is the stop motion version:

When you select the geometry, and choose Copy, everything is the same as what I showed:

However, when you then choose Exit Sketch, the geometry you copied is still selected:

Further, when you choose New Sketch, the geometry is also still selected:

And, New Sketch says "oh, something is selected, I'll try to make a sketch plane out of that stuff".  So, it chooses a sketch plane based on that selection.  Because the order in which the curves and points are selected is somewhat random when you use window select, you will get varying sketch planes defined.

So, the solution here is to just click in space after you have selected Copy, to unselect the geometry.  Then, when you start a new sketch, you will get prompted to select a plane.  Choosing the same plane as the one your source sketch is based on will always create a sketch with the same coordinate system, and things will be oriented as you expect when you do a paste.

Jeff

[OFGLLC]

It's funny, I never received an email of your post.  I was going in to update my own question.

I think it's possible that your solution is what we were doing sometimes although the selection is on the same plane.   Most of the time we create the new sketch before ever selecting or do the copy from the new sketch of a displayed sketch, so it isn't a total solution but I determined that if we leave the light bulb on for origin and always create new sketches when in perspective mode. we always see the plane selector and always select the Z plane and haven't had a problem since that.  I wanted to test it for a week to be sure.  I'm not sure at which point Fusion loses it's reference to the only plane we are using but I think you are correct that it does.

thanks,

Jeff

PS, Now for fun, solve Episode 1 and you will really deserve Kudos.  Hey, I better go check if anyone did!