This is a very simple situation; one that is fairly easy to work around, but I don't understand the need for extra mouse clicks.
I'm wondering if I'm just missing something.
ZW was the CAD software we used to use. In ZW you could click on the view you needed to sketch from and when choosing the datum that was parallel to the screen the placement of the sketch did not move. For sanity's sake I like to view a sketch from it's logical direction.
I'm wishing the same thing was possible in Creo (Perhaps it is, but I've not got this to work with the FRONT VIEW sketch)
My views and datums are not the standard Creo orientation. I've changed this to the World View Coordinate System.
This is how the view orientation looks lined up with the datums.
Let's say I want to make a sketch from the Front View.
1) I set up to be in the Front View.
2) I pick the Front Plane. BELOW IS THE ORIENTATION I WANT TO END UP WITH.
When I do 3) select Sketch it completely flips the view orientation as shown.
I can get this back to the orientation I WANT TO END UP WITH but it takes a couple additional sketch orientation steps. I need to Flip Section
After this I need to Flip Sketch Plane and it is back to the ORIENTATION I WANT TO END UP WITH.
As stated above this only doesn't work with the FRONT VIEW. If I go into a template that I didn't change to World View all 3 main directions work with the sketch orientation.
I can get the FRONT VIEW sketch to fall in it's true position if I don't select the Front Datum prior to selecting sketch and flip the arrow so it is pointing down instead of up as follows.
Everything else appears to be correct with my View and Datum orientations, they act like they should.
Does anyone have an idea of how I could by default get the arrow to be flipped to aim into the screen without having to select this manually? I think this would prevent the flipping and rotating of the FRONT VIEW.
It's hard to tell specifically but I think what is happening is your preferred sketch orientation is on the "back" side of the front_local plane.
Planes have a front and back that you can see with the brown? and black? color (used to be easy to tell red and yellow).
I believe Creo is trying to assume you want to sketch on the "front" side of the front_local plane. I'm not sure there is a solution. Possibly a mapkey to do the selections for you based on names of the planes.
You should be able to edit the definition of the FRONT_LOCAL plane and flip the "normal direction". That should take care of it.
Dave: I like this idea but when I Edit Definition to the Datum it appears the Normal is in the correct orientation without flipping it.
Are you sure that's the right way? The normal shows the 'front' of the plane; this is opposite to the default direction of viewing on that plane. In different words, when you sketch on a plane the Normal arrow will be pointing at you, out of the screen.
This is correct. The arrow points out of the screen when sketching. Just try it and start a sketch and it should orient correctly.
Stephen: It appears the Normals point the direction they should. I am seeing all my normals Brown in the positive direction.
The only thing mixed up so far appears to be the Sketch Orientation.
You are right Dave; this does work if you flip the Front Datum orientation.
I like the fact that this works however I'm a little hesitant to make this change unless I'm sure it won't mess up anything else that I've done.
This would have it's normal pointing in a negative direction whereas the other primary datums are pointing in the positive direction.
I will definitely consider this if it wouldn't create other issues.
your template of part have a wrong front view definition. y axis should facing outside not inside the screen.
click manage-views/view manager/orient/front/redefine
change front to back in the frist reference, choose front datum , choose top as top,
so you will get what you want, the defaut view from ptc.
This is one of those things that has bugged me forever. If you're used to a "z-up" world and set up Creo accordingly, you have to manually change the sketch direction every time you pick the front (x-z) plane. Technically this makes sense since you're seeing the back of the plane, but Creo should be smart enough to set the viewing direction based on the direction you're currently looking at the model. If I really want it to rotate the model 180 degrees then I will manually flip the viewing direction.