changing sketch orientation

[icreator3d]

G'day all,

Does anyone know if it's possible to change the default sketch orientation, so that when making a new sketch on the XZ or the YZ planes the Z axis would act as the X, not the Y?

Hope that makes sense.

Thanks

[JDMather]

You could go into Tools>Application Options and set the plane you want to start new sketch on - or do as I do - and set it to No New Sketch.  That you you decide what plane you want to start your first sketch on.

[icreator3d]

Not quite what I meant. 

When you start a 2D sketch on the XZ plane the sketch is rotated such that the Z axis becomes the Y axis.  Is it possible to change settings so that the Z axis will default to being the X axis (instead of being the Y)?

[rdyson]

What happens if you create a sketch with the desired orientation in your template.

Would obviously only worik for the first sketch, though.

[johnsonshiue]

Hi! If the orientation is critical to you, there are two options to consider. One is to use UCS to define the coordinate system in the way you like. The other is edit the Sketch Coordinate system after you creat the sketch (finish sketch -> right-click on the sketch in the browser -> Edit Coordinate).

Thanks!

[icreator3d]

I don't want to change the orientation of the part.  I just want to change the way the sketch appears on my screen while I'm working on it.  I think in Solidworks and ProE, every time you start a sketch you define a relative coordinate system for that sketch, but Inventor picks it for you. 

But judging by the answers so far, I suspect that the answer to my question is "no". 

Thanks y'all. 

[JDMather]

I work in Inventor, SolidWorks and Pro/E on a daily basis.
Never given this a second thought. 

I haven't even figured out what your problem description really is?
I've never worried about a "coordinate system".

[swalton]

My guess is that the OP is like my boss.  He wants us to sketch in a consistent manner.

Pro-E planes are labeled TOP, RIGHT, FRONT.  He wants us to model the parts so that each sketch uses those planes in a consistent manner.   If your first sketch uses the top plane as the horizontal reference, all sketches on any plane that is normal to the top plane should use the top plane as the horizontal reference.  In ProE, selecting the sketch horizontal and vertical references is part of sketch setup.  Sure, ProE makes a guess as to what you want, but you can override it before entering the sketch environment proper.

IV requires you to exit the sketch, before placing any geometry, and then redefine the sketch origin to follow a consistent horizontal and vertical scheme.  Lots of extra time and interrupted workflow for a nice-to-have, not a have-to-have feature.

[JDMather]

---

@swalton wrote:

 He wants us to sketch in a consistent manner.

  He wants us to model the parts so that each sketch uses those planes in a consistent manner.  

IV requires you to exit the sketch, before placing any geometry, and then redefine the sketch origin to follow a consistent horizontal and vertical scheme.  Lots of extra time and interrupted workflow for a nice-to-have, not a have-to-have feature.

---

I thought I was being consistent across all three programs without any special effort.

[swalton]

I guess what I mean is for a sketch on any plane where the positive direction of the origin y-axis could be up, relative to my monitor, how do I ensure that IV makes that axis up when I pick the sketch plane? 

[JDMather]

I never worry about it.
Most of the time I start out a sketch (2D) from a 3D perspective as I live in a 3D world and that is how I think.  (in fact it irritates me when Inventor swings around to a parallel view when starting a sketch and I have to nudge my Space Navigator to get back into a 3D perspective on what I am modeling.)
Once I have a few enitties I might clcik on the glass cube and rotate if needed to finish up the sketch from a 2D perspective.

[swalton]

Functionally, I agree with you. 

In IV we don't care either, because it is too cumbersome to control.

But, in ProE, where the company owner/head engineer will review your work, and he wants up to be up in each sketch, we care.  He signs the paychecks. 

[JDMather]

---

@swalton wrote:

But, in ProE,  

---

Show him Ctrl Wheel in Pro.
My sketch is going to be oriented correctly relative to the rest of the model - no matter what plane I select as Reference.

[udayag]

One possibility is to have a customized part template with two additional workplanes (named, say, "my XZ Plane", "my YZ Plane").

To cretae "my XZ Plane", first create a sketch using the "XZ Plane". Then using the "Line" command first pick the origin point (point A), then pick a second point (point B) so that AB is vertical. Note that AB is parallel to the Z axis. Pick a third point  (point C) so that C is to the left of line AB. Now create a workplane based on 3 pounts and pick the points A, B, C in that order. Rename this workplane as "my XZ Plane". DElete the sketch you created earlier without deleting the dependent workplane. You could create  "my YZ Plane" similarly.

Any sketch based on these workplanes will be oriented the way you desired.

Save this part file in the template folder with an appropriate name. 

[Patrickwesc]

Let me guess, you're a cut, extrude and mate kind of guy.......

[5103141590]

You can turn off normal to sketch in application options under sketch tab - "Look at sketch plane on creation"

[alokkY488N · Accepted solution]

Hello sir,

Even I had the same issue and as Johnsonshiue sir said, "Edit coordinate system" can be used to change the orientation while sketching just like sketch orientation in creo. I have attached the recorded screen of using the command and would urge you to go through it.

Thanks & Regards

Alok Kumar