Tan.Le---Using the datum axis or point only works in the extrude feature. Does not help with a revolve feature.
Sokheng---Adding a point to the drawing puts an X on the drawing for the centermark, not a true + sign.
Is there a way then to put a centermark on that circle/slot center etc.? I know how to dimension to the center, but if you don't put a centermark, then it looks as though your dimensioning to a random spot on the drawing. I don't want to have to add anything to the model and then show it in the drawing (then make sure all other axis or whatever are hidden), because frankly, that is silly and cumbersome. Centermarks and centerlines are basic 2d drawing standards that should be easy to show. In other programs there would be an icon called centerpoint or centermark that you would just click the circle, arc etc and it would create a centermark. Am I missing something, or is ProE just made to be cumbersome?
I believe what you want is to create an Axis Point while in the Sketch of the slot. This will show up as an end-on axis in your drawing, i.e a "center mark".
In the case of an obround slot (one of the commonest uses for this), just put a centerline through one of the arc centers parallel to the slot extent, and another perpendicular centerline through the midpoint of the straight side, and an Axis Point at their intersection.
It's impressive how complicated is a simple thing, like to put a center mark, in Creo can be so much complicated. In Autocad, Inventor and solidworks is just a simple button...
If anyone can make a tutorial to make a center mark in the drawing without doing it by "hand" please let me know. I will apreciate.
Thanks and best regards
Assuming you are trying to dimension to the centre of an obround, this is the easiest way I have found:
Open the Sketch of the obround feature for editing. Draw a diagonal line from one end of one of the straight lines of the obround to the opposite end of the other straight line. RMB, Convert to Construction. Sketch, Axis Point at the Midpoint of the construction line you just drew.
Now, when you show the axes of the obround feature in the drawing, there will be one at the centre of each radius and one in the middle of the whole thing.
I hope this makes sense. If not, feel free to ask.
Here is what I found. Under the "Annotate" tab, select "Show Model Annotations" and a dialog box should appear. Select the right most tab on the box titled, "Show the model datums". Click the feature you want a center mark for, and then click the check-box tab in the dialog box; this will add your center mark.
While we're on the subject, you can also turn on the option to have extrusions with less than full rounds generate an axis.
config.pro - show_axes_for_extr_arcs yes
If you are a minimalist, you won't like it, but if you need it, it can be created by default.
We want to dimension from the end face to the centermarks of the radii in this item, in order to show where the arc center is located. How do we show them? This is a revolved feature creating this cylindrical part.
Is this in the model or in the drawing?
If it is in the drawing, you can shown annotation and have the centerline of the cylinder (right side) or the center mark of the endviews (left) show up as selected.
As shown below, A_1 is selected and shown up in yellow. The rest in red haven't by selected. Then either hit apply or OK.
Dale, this is the result of a work around that I was creating, but found out the hard way if someone responds to your post, it is no longer editable??>. LOL
These results can be accomplished by creating a seperate sketch on the viewing plane, using Project on the sketching tab, referencing the radii, then adding vertical DATUM centerlines to each centerpoint, and add horizontal DATUM centerlines to EACH centermark (these will overlap here), then accept the sketch, return to drawing, and Show Model Annotations to show all axis/datum lines for the features. You may now use the grips on each centerline to adjust the sizes of the datum lines. If necessary, you may make your view INDEPENDENT from the drawing and hide the sketches; it will leave the "centermarks" alone.
From the revolve itself, there should be an axis that you could show through the annotations both the longitudinal axis and the centermarks on the end view.
This is an unusual case for requiring the center cross-hair. You can either sketch them (high pain level) or you can add geometry point in the revolve sketch. You can define a datum axis through the geometry point. You have to know that your orientation of the sketch will coincide with the drawing as expected. There is no clean way to do this until PTC sees that having optional center cross-hairs should be part of the dimension leaders, not just axes.
Use sketch to make points. Use those points to make axises. On the drawing, use show model annotations to show axises (centermarks).