15-Moonstone

Question

Logic behind Sketch Orientation?

Forum|Forum|10 years ago
October 6, 2015
6 replies
18918 views

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.

Datum Orientations.JPG

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.

Front View.JPG

When I do 3) select Sketch it completely flips the view orientation as shown.

Front Sketch.JPG

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

Flip Section.JPG

After this I need to Flip Sketch Plane and it is back to the ORIENTATION I WANT TO END UP WITH.

Flip Sketch Plane.JPG

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.

2D Drawing

S

StephenW

23-Emerald III

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.

P

pimm

Author

15-Moonstone

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.

D

DaveHeipel

1-Visitor

You should be able to edit the definition of the FRONT_LOCAL plane and flip the "normal direction". That should take care of it.

P

pimm

Author

15-Moonstone

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.

Normal Direction.JPG

J

JonathanHodgson

13-Aquamarine

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.

C

claudedubois

1-Visitor

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.

T

TomU

23-Emerald IV

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.

C

claudedubois

1-Visitor

have you try the way to make your orientation the way you like. in fact, whtn you use extrude , remember to extrude to the other side then defaut, after you have all views as it should be in drawings.

B

BrentDrysdale

12-Amethyst

Hi Paul,

I am another loooong time user of ProE (Creo). It has been a while since I was on the forum but lets see if I can add anything.

Creo uses a default set of assumptions which happens to be based on the old paper drawing board (as do some other systems)

This means that X is horizontal to the right of the screen as if you look at a drawing board and Y is is up the screen. By the Right Hand Rule for Cartesian coordinate systems this makes Z coming out of the screen at you.
Thus the Front datum plane is the XY plane and it is the drawing board view. In the old ProE methodology this is the positive (Yellow in those days) side of that plane; the opposite side of the plane is negative (the Red side). Top datum plane is the XZ plane with the positive side facing up (again Yellow) and the negative side facing down (Red). Lastly the Right datum plane is the YZ plane with positive (Yellow) facing to the right of the screen (drawing board) and the side on the left is negative (Red).
When you are in your 3D view of your part and you pick the Front datum to sketch on (to Extrude) Creo will default to using (from memory) the Right datum as a reference AND it will orient the sketch so that the positive (Yellow) is facing you (out of the screen and with Right Datum vertical and with positive (Yellow) to the right no matter which way you are looking at the part.
- And the extrusion direction will be in the positive direction.
- This is entirely logical though it can be disorienting when:
  - you think that the Extrusion should extrude away from you but it comes towards you. There is an arrow that tells you the direction BUT you cannot see it properly in 2D. Towards you it looks like two small concentric circles (supposed to be the tip of an arrow) and away from you is an X (supposed to be the tail-feathers of he arrow).
  - your part spins around to present your sketch flat on to the screen. Personally I disable the automatic alignment of sketch to 2D and I usually sketch in 3D. Also helps with that you can now see the extrusion direction arrow. Personally I loathe Trimetric and use Isometric instead so the Yellow (positive) sides of the Datum Planes are facing you by default but you choose your poison.
BUT if this Creo set-up doesn't suit you when you are making parts for some reason then the answer I have not seen discussed is to set up your template part and assembly with the orientation you want. Two ways to go about this:
- Make a blank part (not using a template) and add default datums. Rename those suckers how you want. Add a coordinate system by picking the three planes and fiddle the orientation of the CYS till the XY and Z point the way you want them. I do not recommend this but it is possible.
- Or you could live with the default planes and Coordinate system and add and extra CYS that conforms to your World View (gosh that takes me back to AutoCAD in the eighties) and add your own named Views that suit this orientation and save this to use as a template part (and one for Assembly) so it is always that way for you. You then get your supplier to use the added CYS. This would be my recommended approach.

Good Luck.

Regards, Brent Drysdale

P

pimm

Author

15-Moonstone

Brent,

You describe the default Creo views and datums very correctly.

I have successfully set up my views and datums to make sense in a true X, Y, Z environment. Most of this setup works just the way I would want it to. When I extrude from the main datum directions it extrudes into the positive quadrant, there are no surprises with that or my views.

What I would like to see is when I select the front plane, go into the front view and choose sketch to have the sketch orientation not rotate and flip around. This does work correctly with Creo's default datum setup, but for our work environment this doesn't work well.

The flipping sketch orientation is a minor issue which has work arounds. I just wish there was a way to change that one aspect without altering any of the rest of my view or datum setup.

B

BrentDrysdale

12-Amethyst

Hi Paul,

Try setting the option in your Config so that Sketching does not orient to 2D. Can't remember the option name but it is something like;

Reorient Sketcher to 2D with the default Yes

If you try it for a while you may like it

I am happy to use the default plane orientation but then I have used it for so long it just seems normal. If I need some other reference system for discussion/export to a third party I just add another CYS to suit that and more named views that I can use in a drawing if required. PCB export to an ECAD package is such an example but could be that sheet metal or making a 3D print from a simpler 3D printer sometimes needs this too.

Regards, Brent

C

ckeller

1-Visitor

The way I remember the default orientations is to imagine I'm facing an object such as a computer screen. The front faces me, the right side is "my" right. the top matches my up. Also X grows to the right, Y grows toward the top, and Z grows out the screen toward me. (for the defaults) (order of rotations follow right-hand-rule. if Z is your thumb, X is your index finger, and Y is your middle finger. (XYZ, YZX, ZXY - from thumb-index-middle) and the rotation around the thumb axis is in the direction you'd fold your fingers to close to a fist.

Automatic Sketch Orientation (in my experience):

when you choose a datum plane to sketch on creo does 3 things:

1) sets the sketch so that the plane normal is facing toward you.

2) sets the up-direction such that the datum plane moves the least. in other words, if you had the plane you were choosing in the exact position you wanted to start sketching, it won't rotate at all.

3) sets the sketcher orientation reference to the first available datum plane. and chooses the orientation mode that matches the creo-decision made for step 2.

Assume the default 3 datum planes from the standard mmns_solid.prt template that ships with creo. Datum Plane Order is RIGHT, TOP, FRONT.

if you choose "RIGHT" datum plane to sketch on, creo will rotate the sketcher so that the datum's normal is pointing toward you, as close to the same orientation as you had. Then will use the "TOP" plane as the orientation reference.

For your first example you are not actually asking for a front view. you are looking for a front-facing view, which is the back view of the object. That is, you are looking forward as if you were the object, but in actuality since you are outside of the object, and looking at it, you are looking at it's back side.

So for your example, you choose the "FRONT" datum plane and if creo defaults to using the "RIGHT" plane as your orientation, when you "flip" the orientation it will turn your sketch plane upside down while flipping it. If instead you move the TOP datum to the before the RIGHT datum plane, then when you "flip" the orientation it will rotate your sketch plane around the vertical axis because the orientation reference would be the TOP plane instead of the RIGHT plane.

as: