topic Re: Sketch Projection Not Working/Updating Properly in Fusion Support Forum

Sketch Projection Not Working/Updating Properly

clementPLHPN — Thu, 18 Feb 2021 20:50:57 GMT

Hi there and thank you already for your help.

I'm kinda struggling with the projection feature of Fusion 360 in general, but now it is just not working...
If you look at my CAD (which I simplified) you should be able to experience similar issues.

ISSUE #1:
Changing any dimensions to Sketch "Front" is not reflected on Sketch "Offset", which is supposed to be a simple offset line of a projected edge.

I tried "Compute All", going back and forth in the design history, fixing the "Offset" sketch...nothing helped.

ISSUE #2:

If I change the Sketch "Front", then I can't use the offset feature on Sketch "Offset" anymore. (Try deleting all the lines in Sketch "Offset" and rebuild it using an offset of the projected edge like built originally > I can't)

"SOLUTION":

Change Sketch "Front" > Create a new Sketch "Offset 2.0" using a new projection > Update Extrude "Cut" > Delete old Sketch "Offset 1.0", which is a terrible workflow, especially if you have many things link to those features later on (other projects, other offsets, fillets,...) > You have to rebuild everything which basically discards the parametric logic 😑.

So please let me know if I'm doing anything wrong because I'm a huge projection/reference user, but I keep running into struggles...10 years of Solidworks workflow before switching to Fusion so maybe I just need to re-learn the process...

Thank you 🙏

Re: Sketch Projection Not Working/Updating Properly

g-andresen — Thu, 18 Feb 2021 21:37:33 GMT

Hi,

There is no reference of the profile in sketch "Offset" via a projection of the body contours to sketch "Front".

Therefore, there can be no effect on changes to "Front".

günther

Re: Sketch Projection Not Working/Updating Properly

clementPLHPN — Thu, 18 Feb 2021 22:06:16 GMT

Thanks for your reply @g-andresen .

Please correct me if I'm wrong but it sounds like you're saying I should create a reference of the projected edge in Sketch "Offset" and then offset that projected line, right?

I updated my CAD file (let me know if you can access the latest version):
Sketch "Offset A": Supposedly incorrect, I was directly using the offset feature on the front edge, assuming it would create a reference automatically. (For some reason, some reference points are created tho 🤔)
Sketch "Offset B": I created a projection of the front edge first, using the regular "Project" feature. And then I created an offset of this projected line.

Still running into the same issues...so were you saying I was doing something else wrong?

NOTE: On different files, I recreated all the offset sketches after changing the main one, at first I thought it fixed it because I could update dimensions on sketch "Front" without breaking sketch "Offset" but then I realize it only worked with some type of changes and would react differently after restarting Fusion... > veryyy random issues...
Actually, on the updated file I shared, on sketch "Front" if you decrease the diameter of the side arc (452 to 300), it would update properly. But if you increase the diameter (452 to 500) then it breaks...

Re: Sketch Projection Not Working/Updating Properly

davebYYPCU — Fri, 19 Feb 2021 01:05:47 GMT

I think there are various Project meanings within your file. (latest with offset B fully constrained whilst Front sketch remains unchanged, changes breaks the sketches.)

You would need to define what you want to do.

(As a demo file has some interesting outcomes - prompting a small Rant)

The fillet on the Loft, transfers to both subsequent sketches as Splines. Unconstrained splines, can allow weirdness you are seeing.

Offset Sketch A has no offset dimension, but the mirror in Front Sketch is transferred in. Outline profile is projected by preference setting. (single profiles - see below)

You say that you projected the outline into Offset B, purple lines, correct, then you offset the outline for the black internal profile, all good, except when you created the sketch (on the face of the body or Sketch A profile,) it too was projected by Fusion and the outline curves are purposefully hidden to avoid clutter, but doesn't avoid confusion.

Select Other on the Offset B blue shadings, and you will find two profiles listed, where we humans think and expect there should only be one. ( @jeff_strater you listening? Create sketch on body the immediate light blue shading is not obvious, (unless you hide the body,) I am used to this now but OP has not even figured it out yet.)

Now because Fusion has two / three profiles and splines to play with you lose control of the file.

Two choices, either create sketch on Offset / Origin planes or don't project twice.

Might help....

Re: Sketch Projection Not Working/Updating Properly

jeff_strater — Fri, 19 Feb 2021 04:34:17 GMT

@davebYYPCU - good point. The good news is that, after who knows how many years, we are in the process of, at least optionally, not hiding those auto-projected geometries in an upcoming release. This will be much better, IMO...

Re: Sketch Projection Not Working/Updating Properly

clementPLHPN — Fri, 19 Feb 2021 02:43:01 GMT

Thanks @davebYYPCU for all those details. I'm a bit confused by some of it, so I'm gonna try to navigate through it.

Note, Sketch "Offset A (error)" was broken without me noticing it. Looks like it breaks if I change the reference... I rebuilt the Sketch (Offset A (good)) as originally intended: Start Sketch > Select Front Face > Offset Line Feature > Select Front Edge > (Dimension) > Done.
As opposed to Sketch "Offset B", where I project the front edge/profile first, and then offset the projection.

I think there are various Project meanings within your file. (latest with offset B fully constrained whilst Front sketch remains unchanged, changes breaks the sketches.)

You would need to define what you want to do.
(As a demo file has some interesting outcomes - prompting a small Rant)
I'm trying to make sure that if I only change dimension on Sketch "Front", the changes occurring on the 3D geometry will be reflected in the projection I create in other sketches (≠ breaking)

The fillet on the Loft, transfers to both subsequent sketches as Splines. Unconstrained splines, can allow weirdness you are seeing.
Not sure I understand why those would be considered unconstrained splines? But maybe you're talking about the broken sketch "Offset A (error)".

Offset Sketch A has no offset dimension, but the mirror in Front Sketch is transferred in.
Once again sorry if the sketch "Offset A (error) was confusing.
Outline profile is projected by preference setting. (single profiles - see below)
Couldn't find anything in the preference settings.

You say that you projected the outline into Offset B, purple lines, correct, then you offset the outline for the black internal profile, all good, except when you created the sketch (on the face of the body or Sketch A profile,) it too was projected by Fusion and the outline curves are purposefully hidden to avoid clutter, but doesn't avoid confusion.
Select Other on the Offset B blue shadings, and you will find two profiles listed, where we humans think and expect there should only be one. ( @jeff_strater you listening? Create sketch on body the immediate light blue shading is not obvious, (unless you hide the body,) I am used to this now but OP has not even figured it out yet.)
I think I understand what you're desbricing but I don't understand how this is the issue.

Now because Fusion has two / three profiles and splines to play with you lose control of the file.
Same here, not sure why this is the issue, I mean my reference (front edge of the 3D geometry) is what it is. I should be able to project it 100 times and have the 100 projection update if I change the 3D geometry...

Two choices, either create sketch on Offset / Origin planes or don't project twice.
I sepatered the different ways, plans, profiles and sketches to achieve what I want to make sure we understand each other. See below.

So I reproduced the issue I was running into without having my reference and my projection on the same plan/profile, just to make sure that's not what is causing the issue.
Test #2: I only project the front edge of my geometry.
Test #3: I project the front edge of my geometry first (since I realized that I can't directly offset the front edge since I'm not on the same plan/profile anymore), then I offset the projected line to the desired distance.

But when I changed the dimension/design of the 3D geometry reference, Test #2 updates properly while Test #3 breaks, more precisely the projected lines update properly, but the offset of projected lines don't...

Please let me know if you observe the same issue, and if you know why it doesn't work.

Thanks again!

Re: Sketch Projection Not Working/Updating Properly

clementPLHPN — Tue, 23 Feb 2021 04:48:12 GMT

@davebYYPCU @g-andresen @jeff_strater any chance you might have more feedback for me please?

Re: Sketch Projection Not Working/Updating Properly

davebYYPCU — Sat, 27 Feb 2021 07:42:30 GMT

Sorry, with the currently downloaded file, I don't know what you want to do.

There are some unexpected behaviours when changing the 452 dimension. Unexpected in that a set of offset curves don't result in uniform offset geometry.

After the Loft, you have 4 sketches that are not fully defined, and that can give your loss of control. That some do and some don't lose control, can probably be explained, but your file is confusing to me because I didn't make it, and as said don't know what is required.

Blue / Orange lines are not fully defined,

Black lines are fully defined,

purple projected lines are treated as previously defined.

Might help....

Re: Sketch Projection Not Working/Updating Properly

clementPLHPN — Wed, 03 Mar 2021 01:56:44 GMT

Hi @davebYYPCU,

Thank you for your response and sorry for being a bit late with mine. I spent some time on clarifying things though.

I was noticing random issues on a CAD file I can't share so I tried building simplified CAD files, reproducing the same issues. My goal is to understand why some Projection and Offset features are not updating properly.

I cleaned up and separated my testing files in Test V1 (Extrude) and Test V2 (Loft).
All the sketches are fully constrained (except for one but not sure what's happening there, I'll talk about it at the end).
For each of the CAD you can find 3 bodies: 1) Reference, 2) Extruded Projection of the front face, and 3) Extruded Offset of the Projected front face.
In Test V1 (Extrude), everything is updating properly, unless I change the reference to an extreme that the offset can't manage. But with Test V2 (Loft), closer to my original design, I'm having pretty random issues when trying to change the reference (Sketch "1 - Reference Front"): Height, Length and/or Arc radius.
Basically, the "Projection Only" always works, but the "Projection + Offset" works great on Test V1 (Extrude) but doesn't on Test V2 (Loft)...and I don't understand why...

Last thing, about that sketch that is not fully constrained: Test V2 (Loft) - Sketch "1 - Reference Back"

The arcs are not fully constrained (blue color), even though I think they are, especially since I can't freely move them...no idea what's going on there...

Feedback are more than welcome like always, Thanks!

Re: Sketch Projection Not Working/Updating Properly

davebYYPCU — Wed, 03 Mar 2021 04:45:13 GMT

Working in Test Loft only, as the other one works, not gone there.

Fix sketch 3, by deleting the 2 arcs, redraw the left one, making sure to snap to the end points used to define it, Sketch snap is important, it turns black immediately. Mirror it to the other side.

Then I couldn't break the model after doing that with a range of arc values between 300 and 800 - can't tell you why.

Might help....

Re: Sketch Projection Not Working/Updating Properly

clementPLHPN — Wed, 03 Mar 2021 05:53:51 GMT

Hi @davebYYPCU,

Thanks for the quick response, especially since it seems like my problems are solved now!!
I still don't know how I got my arcs underconstrained and why it was impacting the whole thing, especially because it was on a sketch that I wasn't using as reference; but I guess it was messing with the Loft feature anyway.
I rebuilt everything perfectly, and now I can change any dimensions and see propagation of the changes 🎉

Summary of the different solutions for whoever might read this post later:

Always make sure your sketches are fully constrained. If it's still blue, even if it won't move, it means something is wrong. It gotta be black!
If you have many sketches on a similar plan/face, especially using projection, make sure you use the proper reference, between profiles, sketches, lines...

Thanks again!