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Logic behind Sketch Orientation?

Re: Logic behind Sketch Orientation?

Indeed, it looks like we're just coming at this from different directions.  For me Thomas Braxton pretty much captured it in the other linked thread:

This is why I am still of the opinion that the default datums of start parts should not in general imply orientation in the absence of geometry. There are conceivable exceptions, however start model default datums should not have names like front, top, right IMO.

One work-around I've realised I use, is that I never hit the 'default orientation' button - I always use one of the other named views from our start part.

I also don't understand the issue with orientation when exporting, but then I'm working in automotive and we tend to agree our assembly origin (and orientation) before we start a project.  The default orientation when assembling is simply "X on X, Y on Y, Z on Z" - that makes sense to me.  I find myself more confused by Catia, which somehow appears to manage with no absolute frame of reference in an assembly - everything just seems to float in space!

Re: Logic behind Sketch Orientation?


Tom, "You would think PTC could at least be consistent across their product line" made me laugh a little....then cry. ;o)

Re: Logic behind Sketch Orientation?

Jonathan:

In our case we got spoiled when we got the VX (now ZW) software because the view environment matched the orientation used in the machine shop, and our parts get manufactured in the same orientation.  We have tried to match the same environment with Creo.  (It works with some minor issues, just like Tom has also suggested).

We are a 3rd tier automotive supplier.  Most of our models are received from Catia as well.  We always wish the models could be supplied in the orientation it was built and not the vehicle assembly location.  Some of the parts don't have more than 1 feature that is flat so it is hard to line up for our purposes.

Re: Logic behind Sketch Orientation?

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

Re: Logic behind Sketch Orientation?

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.

Re: Logic behind Sketch Orientation?

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

Re: Logic behind Sketch Orientation?

Brent,

I do prefer going to sketch in 2D.  Even if I start with an orientation more to my liking with 2D disabled as soon as I click on Sketch View I'm out of luck; also the constraints don't reflect what I'm trying to achieve without reorienting the sketch view.

Perhaps after a period of time I might be able to acclimate to the creo view system, but we have at least 10 years of data made to the World Coordinate system.  To go back and forth would be extremely confusing and mistakes and extra time spent would likely be the end result of the confusion.

Re: Logic behind Sketch Orientation?

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:

2017-03-26_13h32_51.png2017-03-26_13h32_55.png

2017-03-26_13h33_03.png

2017-03-26_13h33_08.png

2017-03-26_13h33_11.png

WHEN YOU REVERSE THE ORDER OF THE DATUM PLANES, THE SKETCHER ORIENTATION DEFAULT PLANE BECOMES TOP INSTAEAD OF RIGHT.

2017-03-26_13h33_35.png

2017-03-26_13h34_12.png

2017-03-26_13h34_18.png

2017-03-26_13h34_24.png

NOW FLIP THE PLANE AND TOP STAYS FACING TOP!!!!  (This is the order I have my planes in my start part and it saves me a ton of headache))

2017-03-26_13h34_27.png

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