topic Re: Sketch bug causes dimension/constraint issues in Fusion Support Forum

Sketch bug causes dimension/constraint issues

Sam_Sanford — Sun, 29 Nov 2020 20:44:05 GMT

You can follow my screen recording here to see how I recreate the issue: https://youtu.be/qOhf8Zy9h-8

I can create the bug repeatably and the way it manifests is with the circular pattern sketch tool. Once it is applied, I can no longer adjust the primary dimensions of the line that serves as the backbone. This also happens with the mirror tool as well. The workaround is to just manually create all the geometry.

In addition after carrying on and attempting to finish my sketch, I encountered multiple issues just within the span of a few minutes. See my process here: https://youtu.be/S-SR9zw6HmQ

Am I just missing some fundamental rule or concept that is causing all these errors in the sketch environment?

Re: Sketch bug causes dimension/constraint issues

jhackney1972 — Sun, 29 Nov 2020 21:51:33 GMT

Please attach your model so the forum users can troubleshoot it. If you do not know how to attach your model, open it in Fusion360, select the File menu and then choose Export and save the .F3D file to your hard drive. Then use the Attachments section of a reply forum post to attach it.

Re: Sketch bug causes dimension/constraint issues

Sam_Sanford — Sun, 29 Nov 2020 22:51:30 GMT

Thanks for that tip. I have attached my file....

Re: Sketch bug causes dimension/constraint issues

jhackney1972 — Sun, 29 Nov 2020 23:33:24 GMT

On the issue you created this forum post, I believe is is a Fusion 360 sketch solver bug. Since the model you attached is way past this error, I create a separate sketch to verify. I made a few comments in the Screencast that I hope you take to heart as you continue with Fusion 360. In you YouTube video, you made the comment you could not import Inventor models. If you have a Fusion 360 Personal license, you cannot but all others you can. The thing is they come in just like a STEP or SAT file would import to Inventor, they do not populate the Browser with sketches and features. In Fusion 360 language, they come in a Direct Model entities.

Re: Sketch bug causes dimension/constraint issues

Sam_Sanford — Mon, 30 Nov 2020 00:27:39 GMT

Thanks so much for those useful tips. My takeaways are:

reduce sketch complexity and do mirror/patterning in the model instead.
I botched my feature tree organization and my core part (the arm) is unfortunately floating as a body and not a component as it should be. I very intentionally tried to begin the project by creating a new component and have that be the arm, but I guess I did something wrong there.
I had no idea I wasn't building the models under the main assembly. It looked to me to be okay at first glance because the components are located underneath, but I guess I just made a simple beginner error there. I guess I have do it all over again and do it right?
It sounds like I can import Inventor IPT parts as long as a purchase a Fusion 360 standard license and then I'll be able to direct edit the models too?

Thanks!

Re: Sketch bug causes dimension/constraint issues

davebYYPCU — Mon, 30 Nov 2020 00:43:28 GMT

Your summary is correct,

John took my words before I could open the file.

My comment was going to be along the same lines, as John has made,

What I was going to say was - why the rotational angle concern in the sketch - when assembling four of them later will be an Assembly pattern/s with joint angles as the parameter? Making your angle parameter is short sighted, and created a lot of the solver problems.

Might help....

Re: Sketch bug causes dimension/constraint issues

jhackney1972 — Mon, 30 Nov 2020 00:45:41 GMT

I did a Screencast of the importing of an Inventor 2021 IPT into Fusion 360. I also tried to give you an idea that it is not a parametric component but a Direct Model object. You can recognize features but apart from holes, it is not a lot of help. You can also import Inventor Assemblies but it DOES NOT select all the components automatically, you have to select them manually and if you are not a "neat" Inventor user, that can be sometimes problematic. You can always use an Inventor Pack and Go and get it all together first. Here is want the Import screen looks like for the Inventor assembly containing the part I used in the video. Look below the first graphic to see where the Screencast Recorder is located in Fusion 360 (if you installed it correctly that is). I can send you a link to a video on how to create a Screencast and attach it if you would like. It is too long for a Screencast so I had to do it in Camtasia.

Re: Sketch bug causes dimension/constraint issues

Sam_Sanford — Mon, 30 Nov 2020 01:01:11 GMT

Okay I think I understand my mistake concerning my component organization and why it's all wonky. It appears that I created the arm part as a component under the main file, but the following components (sandwich plate and top plate) I accidentally created as components underneath or nested within the arm component instead of being on the same level. I must have just right clicked on the arm component file and said "create new component" which created a component within the arm, when really I should have right clicked on the very top project icon and selected "create new component" to put the sandwich and top plates at the same level as the arm. That's probably why there was some wonky stuff going on when I was trying to reference geometry across parts for sketching and extruding.