Datum Feature Symbol Help

[navyhill]

I am fairly new to Pro/E and I am having trouble figuring out the process for getting reference datums to display in my drawings. I have defined two datums in my model. A datum plane "A" on one end of a cylindrical part and a datum axis "B" through the centerline of the cylinder. The datum feature symbol displays in the model correctly on their respective datums. When I go to the drawing, the datum "A" is correctly shown on the drawing view, but the datum "B" is not showing up. I have tried inserting every possible view, along with Show/Erase > show all - to try to get Pro/E to display all datums, to no avail. I have also tried placing the datum on the feature itself and attached it to the surface of the cylinder. Again, it shows correctly in the model, but will not show in the drawing. Does someone have a nice little tutorial or some helpful hints on this or even a way to add the feature symbol manually in the drawing? Thanks!

 

[dakeb]

Datum axes don't show/erase as datums on the drawing. They are attached to either a dimension or an axis, which must be shown for the datum to appear.

In the model, right-click the required datum axis in the model tree (you will have already given it a datum letter).

In the dialogue box, select the Datum Symbol type [-A-]. In the placement dialogue, click 'In Dim'. Select the appropriate geometry on the screen, and all the dimensions will appear. Select the diameter dimension you want the datum to appear on.

Show that dimension on the drawing, and the datum symbol will show up.

If you don't want to show the datum on a dimension but on the axis itself, select Datum Symbol type [-A-] and in the placement dialogue, click 'On Datum'. In the drawing view make sure you are showing the correct axis and the datum will appear.

Dave

 

[navyhill]

If I do the procedure that you described to attach the datum to a dimension I can get the datum symbol to appear just like you said. However, if I try to use the other datum symbol (the filled in triangle as per ASME 14.5-2009) it no longer appears. When I click on the other symbol, a message appears that says the current annotation plane definition is invalid for the placement of the annotation. Then it tells me to go change it in the annotation orientation dialog box.

I tried this. I changed the setting to every preset plane in the drop down box (front, left bottom, etc.) and kept getting the same error. Any clue as to how the annotation orientation is supposed to work?

The view on the drawing is from the left hand side, so I thought that was the most logical choice to set as the annotation orientation, but apparently I was wrong.

I guess all of the trouble is coming from trying to use the new datum symbol.

Thank you for your time.

 

[dakeb]

For datum axes, the [-A-] option will appear as a filled triangle in the drawing without selecting the filled triangle symbol.

For flat datums, as I always have datums switched off I tend to first use the [-A-] option to display the datum plane. When the datum plane is displayed select the filled triangle then select the datum plane as the annotation plane.

There is probably more info available or even a better way of doing it, but that works for me, and seems to display correctly on the drawings.

Dave

 

[navyhill]

Thanks a ton. That at least gives me something to go on. I appreciate the help.

Kendall

 

[Alley71]

Hi,
I noticed you wrote:
Show/Erase > show all - to try to get Pro/E to display all datums, to no avail.
I tried to show/erase datums and it wouldn't show but if you show/erase axis it does show. Not sure if you tried it or not but it worked for me.
Cheers