Re-Orient to Sketch Plane

[Zero__]

Hey guys - small issue that's slowly becoming a bigger problem.

Is there a "View Sketch Plane" or "ReOrient to Sketch Plane" command? Sometimes when I'm sketching I'll twist my views around to get a better idea of something or another and then need to resume sketching on the sketch plane. I can't figure out a good way to realign to the sketch plane. In NX there's a "Sketch View" command. One click and I'm back staring at the plane of my sketch.

Sometimes I can get around this using the Plane View Cube (or whaever you call it) in the upper right corner. But this doesn't work when I'm sketching on a tangent plane, for instance. If there's a "sketch view" command I'm missing I'd be grateful if someone pointed it out to me.

Secondary question! When I am creating a sketch, is there a way to not just select the plane, but also the orientation of the sketch, +X and +Y? In NX (I know, I know, it's always 'in NX' with me) when I'm creating a sketch I not only select the face but also the reference directions. Sometimes in fusion I'll select but when I go "into" the sketch it'll flip around in a weird direction I definitely didn't intend, and I'll be forced to sketch upside down.

[Pedro_Bidarra · Accepted solution]

Sketch Palette > Options > Press 'Look At' without selecting anything else and it defaults back to the original view.

[Pedro_Bidarra]

As for skecthing upside down, you can always rotate the sketch using the arrows at the top right of the 'view cube', these arrows rotate the skecth in 90º increments.

Also, the sketch orientation (as appears on screen) is influenced by the POV you were in before entering sketch mode.

[Anonymous]

Hi Phillip, note that there is different behavior between the two Look At buttons (one being in sketch pallete, the other being on the bottom of the screen toolbar.  I mentioned this in this thread and it seemed to help:

http://forums.autodesk.com/t5/design-and-documentation/look-at-not-paning-to-the-sketch/m-p/5693740/...

Jesse

[Zero__]

Thanks guys - I'd tried the Look At button at the bottom of the screen and it hadn't done what I needed it to, but the one in the Sketch Pallette is working pretty well.

Another sketch question before I start another thread - I want to use the edge of a pre-existing body as a reference in my sketch. I'm not being allowed to select it as a reference for my sketch dimension. I'm also not allowed to select a line in a previous Sketch for use as a dimensional reference. This is the sort of thing I'd do all the time in NX, as a sort of fast parametrization. Changing one sketch early on in the history would echo through later ones correctly updating things like a wall thickness I wanted to stay the same.

Is there a way to do this? In the attached picture, I want to dimension the distance of the line in blue to that corner edge. They aren't on the same plane - parallel planes, as the blue line is on the bottom of that body - but that was never a problem in NX. It would automatically take the projection onto the Sketch Plane.

[Pedro_Bidarra]

Sketch > Project/Include > Include 3D Geometry

(The name is misleading as it allows to include 2D geometry also)

[Anonymous · Accepted solution]

What it sounds like you need to use is Sketch > Project/Include > Project, which will create a purple line that is a projection of that out of sketch plane edge, which you can then dimension to in the current sketch.

Regarding using the dimension of a line in a previous sketch as a parametric reference for the dimensions of other geometry, what you need to do is first go is back into / edit the sketch with the desired dimension, and add a dimension to it.  Take note of the name of the dimension (let's say it's d11).  Then in another sketch (can be before or after the sketch in the timeline with d11 !) for a dimension, you can type d11 (or an equation involving it and other dimensions).  An alternative is if you turn on Show Dimensions for the sketch with d11  then in another sketch when typing the dimension for something, you can click on the d11 dimension, therefore avoiding needing to know the d11name. 

BTW, that's really cool you're an intern at the Pier 9 Lab there!

Jesse

[Maowen_Zhang]

@Zero__, about the question you mentioned below, current Fusion doesn't automatically project the edge (outside of the sketch plane). As Jesse said, need to use "Sketch->Project / Include->Project" it on sketch plane first before adding dimension on it. Feel free to post it inideaStation. 

• Is there a way to do this? In the attached picture, I want to dimension the distance of the line in blue to that corner edge. They aren't on the same plane - parallel planes, as the blue line is on the bottom of that body - but that was never a problem in NX. It would automatically take the projection onto the Sketch Plane.

"Include 3D Geometry" is used to create sketch geometry based on the '3d' edge/work geometry/geometries from other sketches. The only difference comparing to "Project" is that "Project" will do projection the 3d objects on to sketch plane, but "Include 3D Geometry" doesn't but keep geometry in original position (leads to a 3d sketch now). 

[Zero__]

Jesse - thanks. Project looks like it will help sometimes, though it's largely not what I want unless it remains associated with the edge it came form (more below). Parametrization isn't quite what I need here, though sometimes I can make it work to suit my purposes. And yea, interning at Pier 9 is very cool. The robotics lab keeps me busy, that's for sure!

Maowen - so in order to use a body edge in my sketch, I have to "manually" project it onto my sketch plane? Ok. But after I do this, is my Projected curve still linked to the edge it came from, or is it disassociated? I'm hoping it is still associated so my sketches will change accordingly if that edge moves. If this is not the case, I will post in IdeaStation. Referencing prior features gets more and more necessary as sketches/models increase in complexity.

Also, if I'm understanding correctly "Include 3D Geometry" has no use unless I'm creating a 3D sketch? It is just how I make edges referenceable in a 3D sketch.

Lastly and unrelated (I should change this thread name to "sketch questions"). After I create an Offset Curve using Sketch > Offset, can I modify that offset without deleting the curve and recreating it? Or has it become a completely disassociated curve?

[Anonymous]

Yes projected geometry should parametrically update with what is being projected.  And including 3D geometry is going to be by definition for a 3D sketch, since you use Include 3D Geometry to "activate" geometry off of the sketch plane. 

The robotics lab, huh, that sounds pretty neat!  What in general are you working on if you don't mind me asking? 😉

Jesse

[Anonymous]

Oh for offset curves, yeah it looks like for now it cannot be updated parametrically.

Jesse

[Maowen_Zhang]

Thanks Jesse!  

@Zero__, not have to manually project body edges to sketch all the time. There are two cases when Fusion automatically projects them when add dimension or inference to them.

1. Create sketch directly on a body's face, then edges on that face will be automatically projected to sketch when add dimension or inference to them

2. For Body edges inside or even outside sketch plane, use "Look At" command to make sketch plane parallel to screen, then able to select them when add dimension, and then Fusion could automatically project them to sketch for you.  (There are some considerations for this behavior that disable selection when sketch plane isn't parallel to screen, but it might be better to remove this limitation. Anyway, alwasy welcome to share you idea or comments about, thanks!)

• 

For sketch offset curves, you're right, it cannot be updated parametrically right now, but it's in our backlog and working in progress, try to keep you updated when it's ready. Thanks for your post and share with us!