Sometimes when I redefine a sketch plane the sketch geometry becomes "fixed" (green lines). Is there a specific reason why this would happen on some files/sketches but not all of them?
Here's a link to the file - https://a360.co/2Uod2fY
The sketch becomes fixed after redefining the sketch plane second sketch plane after deleting the third extrude command.
@ProductDesignOnline - the green/fixed geometry is geometry that, in the original sketch was "projected" geometry. In this case, from the face that the sketch was created on. When you redefine a sketch, that projected geometry can no longer be resolved (the face it was on is no longer there). So, Fusion converts that to "fixed" geometry, assuming that you do not want it to move. If you want this to become "regular" geometry, you can select it and "unfix" it.
@jeff_strater I've been meaning to bring this question up for a while. Why not just convert to lost projection like in other circumstances where the projection is lost? If it worked like this the new feature allowing reselection of lost projections could be used to fix the error or just break link.
Also if I just move to a new plane parallel to the first it shouldn't really break anything.
The worst part about the way it works now is there's no warning that projection are broken and converted to Fixed. I had to make a modification to a design a while ago where I'd made the mistake of sketching on faces that no longer existed, no problem just redfile sketch plane. Now big problem all projections gone, no warning! Most projections were points so not obvious, only noticed when holes stopped updating positions. OK so edit sketch, delete points and reproject, next problem is you then run into the long time bug in the hole feature where if all point are deleted it defaults back to single hole mode not multiple from sketch no way to fix so delete hole feature, leads to more broken features in the timeline.
The lesson I've learnt is avoid sketch on face because if you delete the face you're in for hours of work trying to fix a design. So any chance of tuning up what happens when a sketch plane is redefined, especially now you have the option to fix lost projections?
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@ProductDesignOnline wrote:
Sometimes when I redefine a sketch plane the sketch geometry becomes "fixed" (green lines). Is there a specific reason why this would happen on some files/sketches but not all of them?
Really? For me it fails every time, even on something simple the projections are converted to Fixed. See attached screencast, couldn't get much more simple than this.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@HughesTooling - yes, those are all good ideas, especially now that we have the repair tool. I'll bring them up with the team, to at least get a sense of how difficult it would be to leave these as broken references. Your point about if the redefine plane is parallel to the original plane, just keeping the reference is also good. No promises, but good ideas.
@TrippyLighting I've run into this a lot where I've inserted a part for mould design then later the customer updates the model or wants a new mould with a slightly different version.
I've used the Offset Plane workaround in the past but you need to think a head. What would be nice is some way later to convert a sketch on face into an Offset Plane and sketch, the sketch using the new plane and all references maintained.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@Anonymous wrote:
So actually you can do that and track projections for offset planes but looks like your code is too restrictively loose projections when plane is redefined for a sketch without checking whether old and new planes are parallel. Is it too hard to check that and fix this bug? Can we turn this "idea" to "implementation"?
They don't even need to be parallel. If you create a plane on a face and a sketch on the plane then move the plane to a different face at an angle the projections update. Just seems lazy programming that it fails when the sketch is redefined from one plane/face to another. If you never sketch on a face but always create a plane for the sketch you can work around most problems but I don't really like this workflow.
Note you can create problems if you rotate a plane so it's parallel with the original projections, lines become points for example.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
I asked someone in the API forum for help to create a script that creates an offset plane and starts a sketch on the plane in this post. It's not going to help everyone but if you know in your workflow when you're going to have problems with losing a sketch plane it's very useful. I guess you could just use this all the time and never sketch directly on a face as well.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
