There are two types of coordinate system features in Creo - the normal "Coordinate System", and the "Default Coordinate System". Creo reserves this internal "Default Coordinate System" - that always set the same orientation.
Basically, Creo always needs something to use as a reference. So, the first feature in your tree can either be:
If the first feature in your model (or your "start part") is a coordinate system - it will actually create a "Default Coordinate System", because there is nothing else in the part to use as a reference.
If you want your start part to use a coordinate system with a different orientation, you can define your datum planes first, then create a regular coordinate system to orient it differently.
aka - if you create your "coordinate system" (and then three datum planes), you will get this:
If you create your datum planes first, and THEN your coordinate system, you can create something like this as you desire.
Note how the blue-green-red are matched to different axes than in the first example, and I've simply renamed the datum planes.
However, a VERY important thing to note: even if you create your "first" coordinate system as I showed in the second example.... if you create a "Default Coordinate System" now, it will ALWAYS create it with the same orientation as in example 1, and you will not be able to edit it's definition.
If you ever want to "change" the orientation of the part... one thing you can do is to create a NEW coordinate system rotated from the "Default". Then you can use "Replace Reference" to change all of your features to use the new coordinate system/orientation instead of the old default one (then maybe hide or delete the default... of course, depending on your company standards, etc).
Hope this helps!
i have to match Assembly default position for my vehicle coredinate system which is i have.
its xyz orentation is different from the default.
This will change/replace the views not how the model is built it up from the main/default coordinate system ... this will not assemble the model in the new default orientation ... will keep the same orientation related to the mail/default coordinate system ...
Creo Parametric 5.0 22.214.171.124 release (New version upload has coordinate system oriented with Z AXIS up).
Has anyone else encountered this?
Since we started teaching and writing books on PTC products (1994), the Z axis always projected out from the FRONT datum plane.
Now it goes up from the TOP datum plane.
PTC has finally got it right!
We have always changed our start parts so the +Z is up from the X-Y (top) plane.
The major problem with that picture is that the positive side of the front plane is pointing opposite the positive direction of the Y axis. Based on the coordinate system orientation the gray (negative side) of the front plane should be visible, not the brown (positive) side.
I just installed Creo Parametric 126.96.36.199 and I cannot reproduce this. Here's what I'm seeing: