Sketch Lines Become Green

[travis.true08]

Could some one tell me what green projected lines and dots mean? Are they broken references? This happens over and over with 2 of my sketches. I've had to delete all of them, and re-reference everything twice for both sketches, and it's become very time consuming. Here's an example:

[daniel_lyall]

That means the sketches are locked (fix/unfix command) in the sketch pallet.

Or they have been broken and fixed.

If they are from a svg they are the same.

You can select them when the sketch is active and click on the fix/unfix command to unlock them.

[travis.true08]

I've tried right-clicking and selecting "Fix/Unfix", nothing appears to change, but the action does happen as it appears in the Undo history. The "Fix/Unfix" command remains, so I can continue to perform that action many times without any perceived effect. Is there a way that I can fix these references, or will I have to remove and redo all the references again?

[daniel_lyall]

Can you post a model in that state, It will be the only way to realy find out what is going wrong. to do this Go to File -> Export and save as a .F3D Archive File and attach it to your next post

[travis.true08]

Yeah, it's attached to this post. The Sketches to look at are: "Back" on the Faceplate component, and "PCB" on the PCB component.

[jeff_strater · Accepted solution]

Jumping in here.  I took a look at this model.  In the "Faceplate" component, "Back" sketch you have some overlapping geometry, some of which are fixed.  I would get rid of any duplicate geometry.  In the "PCB" component sketch, these are pretty straightforward fixed sketch geometries, and you can make them unfixed using either the sketch palette or the context menu.

Here is a video:

Jeff

[travis.true08]

Hi Jeff!

Sorry for the late reply. I ended up redoing the sketch, and forgot about this post (I was up 1.5 days when I wrote it). Thank you for the explanation. It really clears some stuff up. I didn't realize that projected edges/curves could be used directly as sketch elements for things such as extrusions. I thought that I still had to add shapes on top of my projected edges/curves if I wanted to use them, but it looks like this isn't the case.

When I re-did this sketch, I cleaned it up quite a bit. I got rid of most of the symmetry constraints in favor of using the Mirror feature to mirror extrusions with the use of construction planes made from construction lines. Most of my other sketches have been cleaned up to reduce the need for redundant sketches as well, but I'll need to go through them again.

This is still a complex sketch though, so I'm going to take Trippy's advice by breaking the sketch up into multiple sketches for the backside of the face. This particular sketch is already losing its completely-constrained status, so breaking it up should help fix that...

[antoniok9911]

What does it mean when my whole sketch in manufacture becomes green ? I'm trying to cut a simple washer and it won't let me 

[daniel_lyall]

It is a locked sketch go into the design workspaces edit the sketch highlight the sketch and click on the lock simble in the constraints fly out it should change back to a normal sketch. 

[g-andresen]

Hi,

how it works

günther

[lindsay.fowler]

That miming doesn't adequately tell me how it works. My green lines occurred after the dreaded "Redefine Sketch Plane"; all the projected (purple lines) turned to that ominous green. Unfixing just made them into blue lines with no constraints at all. This is no good. I want my projected lines to be preserved, without going green like eggs and ham. 

[jeff_strater]

Redefine does not preserve projected lines.  It is set up to handle the general case, where any plane in any orientation can be chosen.  So, to handle these cases, all projected geometry is converted to unassociated, fixed geometry.  You will have to project new geometry, and dimension/constrain to those projected geometries.

[lindsay.fowler]

Hmmm, interesting. However, if the two planes are parallel then there is no need to break the projections. And I would argue, that when you want to redefine the sketch plane, it's because you don't want to have to do the sketch again. The projections should be kept, and if they are not desired in the new plane, well then the user can simply elect to delete them. I see no use for making them unassociated green lines every single time.

[jeff_strater]

Agreed.  It could work that way.  But, there are complications.  None of them would be impossible to deal with, just requires time and effort.  I'm sure that Fusion will get there eventually.  Just a tradeoff that had to be made for the initial implementation.

[zhouquan27]

I've been hoping for a while now that preserving or re-linking the projected geometry would be an option.

Wonder if it makes things easier to implement a way to "replace geometry" (if there isn't one already).

• When someone redefines the sketch plane, the program still breaks all the projections and turn them green.
• Next, the user re-creates the projections (purple lines, and in most cases these would lie exactly on top of the green lines).
• Finally, the new functionality would be to allow the user to replace each green line with a corresponding purple line, carrying over all constraints. Of course in the non-trivial cases this might fail if the source/target geometry are not compatible.

This lets you preserve the general case without trying to be too smart about auto detecting the projections. The user still has to do some work, but less, since making the constraints is typically more labor than making the projections.

[HughesTooling]

If you want really bulletproof designs then never sketch on a face, alway create an offset plane. If you have a sketch on an offset plane you can reorient the plane to pretty much any new face at any angle and the projection will not break! You could run into problems if the plane ends up at 90° to the original so some lines become points but that's about the only one I've found.

Mark

[zhouquan27]

@HughesTooling, this is a good tip, but I'm not experiencing these issues due to sketching on a face.

Agree that sketching on reference planes will tend to reduce the need to "Redefine Sketch Plane", by allowing for changing the reference plane definition parameters.

Consider a scenario where I have a few different sketches on offset plane A. Now my design has evolved and it makes more sense to move one of those sketches to a different offset, while leaving the rest as they are. In this case, it seems I would create an additional offset plane B, parallel to A, and then have to "Redefine Sketch Plane" from A -> for the one sketch.

Perhaps a dedicated plane for every sketch could be a proposed answer here, but that's not something I would advocate or do myself.

We all would benefit from planning the modeling strategy ahead of time, but one of the reasons we use sophisticated tools like these is they allow us to make continuous changes and improvements to the model without having to re-do work that was already done.

I appreciate that not every feature can be implemented at once. I'm not claiming this feature is the most critical, but I do notice that it's missing.

[HughesTooling]

---

@zhouquan27 wrote:

Perhaps a dedicated plane for every sketch could be a proposed answer here, but that's not something I would advocate or do myself.

---

The program I used before Fusion made you do this and didn't even have the option to sketch on faces. I always follow Rule #1 so don't tend to end up with multiple sketches on one plan so for me the problem only occurs with faces. I also know my workflow so know not to create sketches directly on inserted component's faces or parts derived from inserted components. But the fact you can reselect a reference for an offset plane and not break any sketches with projections show redefine sketch plane should just work.

Then there's the other problem where the new plane mirrors or rotates the sketch and you have to just start over anyway. Redefine sketch plane seems to break one way or another 70-80% of the time!

Mark