topic Re: Sketch behavior is inconsistent after update. in Fusion Design, Validate & Document Forum

Sketch behavior is inconsistent after update.

sohnrog — Mon, 10 Oct 2016 13:53:39 GMT

Hello,

I need help with this. When I try to go edit a previous sketch, I can't. Usually, I can just double click the sketch in the browser and it opens up. Now it won't. If I right click on the sketch, this is what I get. see my screen shot.

I can usually copy and paste sketches as well. This seems to be inconsistent now. I sometimes can copy the sketch from right clicking on the browser tree, but at the moment I can't. See the next screen shot.

Also, when I try to extrude a cut, I'm getting a new error message that some profiles failed to create cutting tools. I am making symmetric cuts from the midline to a distance of "all". I get an error message and sometimes the "ok" button is grayed out. This is driving me bonkers because I have to keep doing the same steps over and over and finally, it will go ahead and cut. See my third screen shot.

I appreciate any help you can give me.

Roger

Re: Sketch behavior is inconsistent after update.

jeff_strater — Mon, 10 Oct 2016 14:16:25 GMT

Hi @sohnrog,

As far as I can tell, double-clicking of sketches in the browser seems to work OK. But, another choice is always to select "Edit Sketch" from the context menu shown in your screen captures.

Fusion does not support copy/paste of entire sketches (i.e. when you select a sketch in the browser), and never has. It is on our list of enhancements for the future, but for now, it is not supported. The best way to copy sketch geometry is to select the curves and points of a sketch, copy those, create a new sketch, and paste those items into the new sketch.

Regarding your extrude problems, it's hard to say without the model. If you can share the model, we can take a look at it.

Jeff

Re: Sketch behavior is inconsistent after update.

Beyondforce — Mon, 10 Oct 2016 14:16:27 GMT

Hi @sohnrog,

Will you please try to Compute All and see if it helps. Also, close the file and reopen it after that.

Ben.

Re: Sketch behavior is inconsistent after update.

HughesTooling — Mon, 10 Oct 2016 14:21:22 GMT

I wonder if the sketch is part of a base feature, was the design started from an import of have you turned record history off at some point then turned it back on?

Mark

Re: Sketch behavior is inconsistent after update.

HughesTooling — Mon, 10 Oct 2016 14:30:24 GMT

I think your extrude problem is because you've chosen Full length for the measurement, try Half Length.

Mark

Re: Sketch behavior is inconsistent after update.

sohnrog — Mon, 10 Oct 2016 14:32:11 GMT

Hi Jeff,

I actually have been using copy paste for quite a few months. It is really useful for my current project. I shortens my workflow by several minutes per model.

Here are 2 models. One lets me copy and paste. The other doesn't.

I tried compute all without luck.

By the way, I realize I'm not activating my component when I work. I did this intentionally a couple days ago and it seemed to fix the copy paste issue, but now it seems random. If you can help, I appreciate it.

Roger

Re: Sketch behavior is inconsistent after update.

sohnrog — Mon, 10 Oct 2016 14:34:43 GMT

Hi Mark,

I imported the model as a mesh and converted it to a solid body. I have not created a base feature in the models I'm working with today. I have done it in the past, but it made no difference for the current application so I skipped that step. If you think it is the root of the problem I can try it, but prior to the update, I could do all of my steps without a problem.

Roger

Re: Sketch behavior is inconsistent after update.

sohnrog — Mon, 10 Oct 2016 14:35:27 GMT

sorry. Here's the screencast.

Re: Sketch behavior is inconsistent after update.

jeff_strater — Mon, 10 Oct 2016 14:50:09 GMT

Thanks, @sohnrog, Something @HughesTooling said triggered a realization for me. You can copy/paste entire sketches in Direct Modeling designs (or in Base Features), but you cannot in Parametric designs. I always forget about direct modeling! So, that is probably why it works for some sketches and not others. If you'd be willing to share the model here, we can tell for certain.

Jeff

Re: Sketch behavior is inconsistent after update.

HughesTooling — Mon, 10 Oct 2016 14:54:42 GMT

The first model you are in direct edit mode, the second has record history enabled. Any sketches you created before enabling history will be in a base feature, you will need to right click and edit the base feature in the timeline before you can edit the sketch in the base feature.

Mark

Re: Sketch behavior is inconsistent after update.

sohnrog — Sun, 18 Dec 2016 00:02:15 GMT

Hi Jeff, Thanks for the earlier comment. It has been a while since I worked on this model and I'm still not able to copy and paste the sketch I'd like to (sketch 5). Here's a model that i can't seem to copy and paste. It has a base feature activated. I can copy and paste if I don't activate base feature. Is there a way to inactivate the base feature so I can copy and paste?

http://a360.co/2i1lcTx

Re: Sketch behavior is inconsistent after update.

jeff_strater — Sun, 18 Dec 2016 20:54:50 GMT

Thanks for the model @sohnrog.

Your post poses some very good questions, for which I'm afraid I don't have very good answers, unfortunately. The specific question, regarding sketch5, is that you cannot copy/paste this sketch as a whole because it is a parametric sketch, not a direct modeling sketch. You can copy/paste an entire sketch if it is a direct modeling sketch, but not if it is parametric. I'll explain (well, kind of) why this is the case below, and also how you can effectively get similar behavior with a few mores steps.

There is a lot of good threads out there on the "direct modeling vs. parametric modeling" religious debate. There is this recent one, which is quite extensive, and has insightful commentary by many of the most prominent Fusion users: direct-vs-history-based-modelling. And this also-extensive one: timeline-bs. There is another thread that is more specifically about this sketching issue: help-mr-wizard. Feel free to read those if you have interest in this area.

But, specific to your sketch copy/paste issue: The reason why Fusion blocks this for parametric sketches is that a parametric design has a lot more requirements around associativity than a direct modeling sketch does. Specifically around how the coordinate system of the sketch and any projected sketch geometry react when you copy/paste a sketch.

For instance, here is a fairly simple sketch on a face of a cube. It has some constraints to edges of the face it is on, as well as an orientation with respect to its own x and y axes:

So, what would it mean to copy/paste this sketch, say to the top face of this cube? You can get a bit of a sense of what would happen by trying out the Redefine Sketch command:

As you can see, the placement is less than ideal. Of course, we could certainly define and solve all these problems, but right now, it is not the highest priority task for us. We will probably get to this sooner rather than later, but it's realistically not in our immediate plans.

So, how can you copy/paste a sketch, then? The best way that I've figured out is to copy the geometry you want from the sketch, create a new sketch, and paste that geometry into the new sketch. Then, you have a chance to position it just how you want it. Of course, you will lose any constraints to projected geometry, but you can hook those up afterward, and any guesses that we'd try to make would probably be incorrect, anyway. Here's a little screencast:

Hope this is at least somewhat clearer.

Jeff