Johnathan: The picture in which I am showing the normal direction is showing brown because I am doing an Edit Definition.
The very 1st picture shows the Front Datum with a Grey color.
All 3 main datums point positive in the positive quadrant.
Yep, so your planes all have their 'front' in the +ve axis direction.
What about your views? From your pictures, it seems you want Front to be viewing on the 'back' of that plane - i.e. the +ve Y-axis direction is into the screen. Is this the case for your other named views - are they defined with the +ve X- and Z-axes pointing into the screen?
Paul Imm wrote:
... if I don't select the Front Datum prior to selecting sketch...
I always use the explicit Sketch Placement dialogue (i.e. never select a plane before sketching), otherwise you're leaving Creo to guess what you want to be your top / right / whatever orientation reference. It's good practice in Creo to always know exactly what you're referencing, for every feature.
In our start part we've got round this problem completely by calling the planes X_0, Y_0 and Z_0, and having six views called X_Front, X_Rear, Y_Front, etc. - it's very hard to say what the front, top or right of a shaft, gear or bearing is in any case!
Yes every datum looks into the positive quadrant. If I do an extrude I would expect it's positive to project into the positive quadrant.
As far as views go; if I place an object on a table if I look down on the object it would be considered the Top View. If I look at the closest edge surface from the front of the table it would be considered the Front View. If I look at the closest edge surface from the right of the table it would be considered the Right View.
The way views and datums are set up you always would look at what is closest to you and an extruded sketch would always extrude into the screen.
I'm sorry if my terminology is deficient. I'm not sure what +ve would refer to.
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.
Sorry, "+ve" and "-ve" are shorthand for "positive" and "negative". I thought that was a standard abbreviation.
Your original problem seemed to be that 'Front' behaved differently to the other two views ("As stated above this only doesn't work with the FRONT VIEW."). If you compare the plane front/back side (normal direction) to the CS_LOCAL axis directions, are all three aligned the same way? I.e., are all three plane normals pointing in the same direction as the corresponding csys axis? If not, then this is why Front behaves differently, and the solution is to make all three orientations the same.
Regarding extrude directions, from recollection I think that the default direction for 'additive' extrudes is out of the screen when viewing the sketch (so the opposite of the sketch viewing direction); for cuts, it's into the screen (the same as the sketch viewing direction). But this is not necessarily the same issue as the sketch viewing direction.
(Your definition of the directions seems a little meaningless to me, btw, because I can place an object on a table any way up I like... the view directions in this case are locked to the object, so this doesn't help! You also haven't said how the axes are oriented to the table.)
Jonathan: I believe what we are both saying is correct but are from the perspectives of opposing coordinate systems. I set my datums and views up using the World Coordinate System and Creo uses the Right Hand Coordinate System. I think both of us are scratching our heads in understanding where we are coming from but when I look at Creo's default coordinate system and apply what you say to it, suddenly this makes sense. I'm not sure why people like working with this type of coordinate system, but if you were using this type of coordinate system it would be difficult to transition out. Since most of the CAD world works in a different coordinate system my viewpoint is going to be a minority opinion, but it works great for seeing things in their true position.
I did submit a Idea Submission in regards to having a choice for World Coordinate System which might resolve the issue I've brought up with the Front View Would like World View model display option
I'm going to try a couple tweaks to my template model to resolve the issue, but I'm thinking I'll just have to deal with it.
Technically both have the same coordinate system (right hand), but PTC has chosen to name the planes associated with each direction differently. Practically this means the PTC default looks like a "world coordinate system" tipped forward 90 degrees.
World CS (z up)
PTC Default (y up)
Again, by simply rotating the model to a z-up position, you can clearly see the CS really is the same, it's just the plane names that are different.
By the way, the z-out and y-up comes from 2D land (before 3D existed) and continues to this day in several different CAD platforms.
Now, while you can create a proper z-up start part with proper views, not everything inside Creo can be adjusted to look right. There are still issues with shadows going the wrong way when viewing shading w/reflections, etc.
Just for fun, here is a link showing Creo users are not the only ones with this issue:
(What will really mess with your head is the fact that Windchill's default for thumbnail creation is Z-up. You would think PTC could at least be consistent across their product line.)
That is an interesting read Tom.
This does show that users would like to have the option to have the X and Y on the table with the Z direction pointing up.
You are correct that when CAD was introduced it was a 2D world and at that time there wasn't any issues related with having Z up on the screen. When it became a 3D world it created the complications.