topic Snapping to reference points in sketching breaks in Fusion Design, Validate & Document Forum

Snapping to reference points in sketching breaks

jamie.q.white — Tue, 29 Mar 2016 18:32:13 GMT

Cursor does not find reference points on hover (center of cylinder, endpoints of lines, edges, etc).

Here's a screencast.

http://autode.sk/1Sks8pI

Design does not matter.

Sometimes the functionality returns after re-starting F360.

Problem has persisted through many versions over years, now. How about a fix?

Thanks,

-jamie

Re: Snapping to reference points in sketching breaks

James.Youmatz — Tue, 29 Mar 2016 18:46:56 GMT

Hi @jamie.q.white,

Sorry to hear this has been happening to you! I saw some of your other posts recently, and hopefully we can try to avert some of the pain.

As far as this snapping issues goes, I have seen this before, but it has been tricky to recreate. For example, I don't think I have ever run into this issue personally, on my laptop. I have seen it on other customers computers, and unfortunately I did not keep track of whether or not it was a Mac or Windows (if that even matters). I just tried to recreate this issue multiple times on different designs of mine and could not.

A few things to check however - in your preferences, in the general-design tab, do you have Auto-Project geometry selected? Do you ever notice it toggling itself on/off?

Also, as a workaround to that issue, does going into the sketch menu and selecting Project and then selecting your cylinder allow you to snap to it? Or if you go into the Construct menu and select point at center of cylinder?

Thanks,

Re: Snapping to reference points in sketching breaks

Anonymous — Tue, 29 Mar 2016 19:13:47 GMT

Hello @James.Youmatz

I have found this happens if you delete a large section (or even all) of your sketch. This may point to the cause. Not sure if this applies to Jamie's situation as well?

Once you lose snapping, it never comes back. You HAVE to delete and recreate the sketch.

I have attached a screencast showing my reproduction of it (I can reproduce it in this manner 100% of the time if the sketch is created on a face)

Workflow for reproduction:

- Create a sketch (it can be on a face, this always fails. If it is on a plane, it only sometimes fails, not sure why).

- Create shapes and see you can snap

- Highlight entire sketch (while still in sketh mode) and press "delete". While in the sketch this should only delete sketch elements.

- try to create new sketch elements - they won't snap!!

At this point, you must delete and recreate sketch to snap again.

Hope this helps you to understand and fix the problem.

Re: Snapping to reference points in sketching breaks

James.Youmatz — Tue, 29 Mar 2016 19:32:44 GMT

Hi @Anonymous,

What is happening in that scenario is that when you window select and delete those entities, you are also in turn deleting the reference that is in place when you create the sketch on the face. (Notice how the yellow profile disappears). This is also the same behavior you would expect in Inventor for instance. In this instance, you will have to go and reproject the geometry back into the active sketch plane in order to snap to the reference geometry. This should work, can you confirm it does?

Thanks,

Re: Snapping to reference points in sketching breaks

Anonymous — Tue, 29 Mar 2016 20:05:13 GMT

I see what you mean, @James.Youmatz.

I didn't notice that was what was happening. You're right, reprojecting the face does let me snap points again.

I still think this is a bit unintuitive (and, I've never used inventor before, but if I had I may have known this).

Perhaps this is the only problem that is happening when I run into sketches that won't let me snap...I will try to project/reproject the elements next time I run into this problem.

Thanks for your help!

Re: Snapping to reference points in sketching breaks

TrippyLighting — Tue, 29 Mar 2016 23:25:14 GMT

I've actually turned the autprojection feature off in the preferences. I prefer control over convenience:

Re: Snapping to reference points in sketching breaks

jamie.q.white — Wed, 30 Mar 2016 12:51:18 GMT

Hi James,

Thanks for the help. I have this issue *all* the time. I've been using F360 for just 20 min so far today and snapping has stopped. It is really annoying and takes hours out of my day, especially when I factor in time spent posting to the forum.

"A few things to check however - in your preferences, in the general-design tab, do you have Auto-Project geometry selected? Do you ever notice it toggling itself on/off?"

Generally yes. Toggling it off does not solve the issue. 3D sketching is on because I need it.

"Also, as a workaround to that issue, does going into the sketch menu and selecting Project and then selecting your cylinder allow you to snap to it? Or if you go into the Construct menu and select point at center of cylinder? "

Sometimes yes, sometimes no for both. Sometimes a re-start of F360 will solve the problem, sometimes I have to shut down and re-start the mac.

Happens all the time. Not just once and a while. Many times per day, over many versions of F360, including clean re-installs off of AD site. Also throught at least 2 versions of MacOS.

-j

Re: Snapping to reference points in sketching breaks

jamie.q.white — Wed, 30 Mar 2016 12:51:47 GMT

Happens in a fresh sketch in a new design. -jamie

Re: Snapping to reference points in sketching breaks

jamie.q.white — Wed, 30 Mar 2016 12:52:59 GMT

I get the problem on or off.

Re: Snapping to reference points in sketching breaks

jamie.q.white — Wed, 30 Mar 2016 12:53:56 GMT

Autumn, I"m glad you got some help but I am having a different problem.

Re: Snapping to reference points in sketching breaks

jeff_strater — Wed, 30 Mar 2016 15:25:03 GMT

One thing I notice, @jamie.q.white, in your original video, is that I don't see the yellow profile that I would expect, once you have started the sketch for the cylinder:

What I would expect to see is more like this:

which makes me wonder: Is the sketch really located on the top of the cylinder? Or is it actually on the origin plane behind the cylinder? The cylinder in that video is so thin that it's hard to tell. That would explain why you cannot snap to the edges of the cylinder. I was able to get a similar effect if the thin cylinder was made unselectable. I didn't see any bodies or components in your model marked unselectable, though.

Can you try this workflow again with a thicker base cylinder, and see whether you get the shaded profile as above, and can clearly tell, by rotating the view, that the sketch is on the top face of the cylinder, and not behind it?

thanks,

Jeff Strater (Fusion development)

Re: Snapping to reference points in sketching breaks

TrippyLighting — Wed, 30 Mar 2016 16:09:02 GMT

Could you share your selection filter settings ?

I am noticing in the video that afte the selection of the sketch plane nothing on the cylinder highlights, whcih is VERY untypical for Fusion 360, where usually everything that could possibly be selected blinks and flickers to indicate it can be selected.

The only time I've seen this happeninng, as Jeff suggested is if either the component is set to "not selectabale", or I outsmarted myself and and forgot that previously I had change the selection filters, which can have a very similar effect.

Re: Snapping to reference points in sketching breaks

michallach81 — Wed, 30 Mar 2016 18:24:29 GMT

I have played with this problem for a while, and I have found that if sketch folder is hidden snap don't work. I'm certain it's just that, take a look at my screencast:

Re: Snapping to reference points in sketching breaks

jeff_strater — Wed, 30 Mar 2016 18:39:43 GMT

Ah, good catch @michallach81! You are correct. This is the problem: The sketch folder is hidden, so you cannot see the sketch geometry, so you cannot snap to it! You can see this (it's a little hard to see because of the Screencast command history) in @jamie.q.white's original video:

The bug here is that there is no warning. If you just create a sketch in this state, you see this error:

but, because Cylinder uses a simplified form of the sketch environment, this warning does not appear. I will file this bug.

Jeff

Re: Snapping to reference points in sketching breaks

TrippyLighting — Wed, 30 Mar 2016 18:46:41 GMT

Exactly! That warning message is the reason I don't hide an entire sketches folder anymore.

Very good catch @michallach81 !

While this is certainly a bug, it generally points to a workflow issue!

Re: Snapping to reference points in sketching breaks

jamie.q.white — Thu, 31 Mar 2016 15:13:42 GMT

Hi TL, thanks fo the help.

"Could you share your selection filter settings ?"

Generally, select all / select through. I've checked this possibility and it does not matter. The function itself stops working.

"I am noticing in the video that afte the selection of the sketch plane nothing on the cylinder highlights, whcih is VERY untypical for Fusion 360, where usually everything that could possibly be selected blinks and flickers to indicate it can be selected."

Well, for me, "nothing highlighting" is VERY typical. I've been working for an hour and had it happen a couple of times. I can usually get around it by creating a sketch, re-sketching or projecting what I need, etc etc. Ugh.

I design bicycles. They have a lot of cylinders: tubes = cylinders, chainrings = cylinders, pedal path = cylinders, wheels = cylinders, rims = cylinders. They all need to be in specific locations with specific dimensions relative to other cylinders. Everytime I need to work around the non-snapping issuse & post to the forums it takes minutes, which x100 per day adds up to hours. It is really frustrating.

thanks,

-jamie

Re: Snapping to reference points in sketching breaks

jamie.q.white — Thu, 31 Mar 2016 15:22:43 GMT

I haven't had time to verify if my problem is the "hidden sketch folder" issue. If it is, then it is a F360 problem, not a "workflow issue", and Autodesk needs to fix it. No error, no UI feedback no nothing.

I need to declutter my design space by switching off sketches within a component. If sketches had Layers (which I requested long ago but as usual no implementation) I could group them to make the declutter easier. If you work differently, that is great, but I can't work that way.

Seriously, Fusion360 guys. Take a few release cycles to get the basics sorted out. This sort of nonesense wastes hours every day.

-jamie

Re: Snapping to reference points in sketching breaks

TrippyLighting — Thu, 31 Mar 2016 15:58:38 GMT

You can turn of sketches to de-clutter your workspace.

You can also turn off sketch folders to de-clutter your workspace. You just have to turn them on when you want to start editing again.

The only bug is that there is no error message. That's an Fusion 360 issue.

Whether Fusion 360 warns you or not, you'll still have to turn the sketch folder back on. Has this stumped me a few times before ?

Sure, but I've learned and adjusted my workflow. That's why I called it a workflow issue.

Re: Snapping to reference points in sketching breaks

jamie.q.white — Thu, 31 Mar 2016 22:56:53 GMT

In some circumstances, placing a cylinder on a surface works ok the first time, but when I try to place a 2nd cylinder on the same surface, snapping to reference is broken.

In at least some cases it is not a simple matter of sketch visibility being toggled off.

I will try to catch it on a screencast when I have more time.

-jamie

Re: Snapping to reference points in sketching breaks

jeff_strater — Thu, 31 Mar 2016 23:51:48 GMT

A screencast would be helpful, thank you. I have not seen a case where you don't get the geometry inferences, but a case certainly could exist.

One small point: If you are doing fully parametric designs, I would recommend staying away from the primitives (cylinder, block). They do not update parametrically, especially for those geometry relations to the sketch. Here is a quick screencast showing this problem/behavior:

in this video, the second cylinder I create, though I created it tangent to the base cylinder, does not obey this if I edit the base:

The historical reason for this is primitives were first envisioned as just a quick way to play with geometry. They were not expected to be building blocks for more complex parametric designs. This behavior is a known problem, and we do plan to fix this.

However, in the meantime, I would recommend that you just use sketch + circle + extrude to make cylinders that you expect to be associative.

I realize that this is not the problem you are experiencing, but it will likely bite you further down the road, so I thought I'd warn you.

Jeff