Options to hide datum plane display using GD&T

I usually convert the standard existing datum planes (front right top)
to Datums A B C.
When I do this, the "plane view" icon does not turn them off.
The only way I can see to do this is to turn the layer off.
Then when I need to use them to constrain the part in an assembly I
have to turn the layers back on.
Is this what everyone else does?
Or is there a better way, or a config.pro setting I can set?
thanks
Reply to
Pete
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are you converting them to geom tols'? I think eometrictolerances r meantto be soemthing other than datum planes
are you converting them to geom tols'? I think g eometric tolerances r meant to be soemthing other than datum planes
cheers Craig
Reply to
craig stevens
I am changing the default Pro/E datum planes into Datums -A- -B- -C-
These are then either shown as free datums, or attached to Dimensions on the drawing.
When this is done, they ALWAYS show on the 3D model. Even when I hide all datum planes.
The only way to "hide" these datums is to blank the layer they are on. Which is tedious
Reply to
Pete
I believe the datums start as DTM1, DTM2, and DTM3. If yours are Front, Top, Right,you must be starting from a start part. This template will have the datums named as you indicated. You can open that template and rename them as you like and they will be that way for ever, and they will turn off when you turn datums off, not using the layers command. Look in you books are help file to see how to make or edit a temlate file. The release 19 books I have explain the procedure, and I don't think that has changed.
Icon that turns that layer on and off.
Mark Janusek Pittsburgh, PA
default Pro/E datum planes into Datums -A- -B- -C-
These are then either shown as free datums, or attached to Dimensions on the drawing.
When this is done, they ALWAYS show on the 3D model. Even when I hide all datum planes.
The only way to "hide" these datums is to blank the layer they are on. Which is tedious
converting them to geom tols'? I think eometrictolerances r meantto be soemthing other than datum planes "Pete" wrote in message news: snipped-for-privacy@posting.google.com... I usually convert the standard existing datum planes (front right top) to Datums A B C.
When I do this, the "plane view" icon does not turn them off. The only way I can see to do this is to turn the layer off.
Then when I need to use them to constrain the part in an assembly I have to turn the layers back on.
Is this what everyone else does? Or is there a better way, or a config.pro setting I can set?
are you converting them to geom tols'? I think g eometric tolerances r meant to be soemthing other than datum planes
cheers Craig
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Reply to
fmc
: I believe the datums start as DTM1, DTM2, and DTM3. If yours are : Front, Top, Right,you must be starting from a start part. This : template will have the datums named as you indicated. You can open : that template and rename them as you like and they will be that way : for ever, and they will turn off when you turn datums off, not using : the layers command. Look in you books are help file to see how to make : or edit a temlate file. The release 19 books I have explain the : procedure, and I don't think that has changed. :
Icon that turns that layer on and off. : : Mark Janusek Pittsburgh, PA : Pete, people seems to be confused (I include myself) about what you are trying to do by changing the names of datums. That's because there are a couple different ways you can do it. You may have used 'Edit>Setup>Geom Tol', thinking this is a convenient way to change datum names. It does a great deal more than that and not being able to 'blank' the datums with the display icons is one small result. The other way to change datum names that doesn't have any drastic consequences is with 'Edit>Setup>Name'. This will let you pick a lot of things, including dimensions, features from the model tree, other datum features besides planes, pattern labels, just about anything with a name or label. If you don't actually need to create geometric tolerance reference datums, it's not necessary, and not a good idea, to do so. If you do need them, it may be a better idea to wait until the end of the modelling process, then rename your datums to geom tol references and identify specifically what dimensions 'get' geometric tolerances. It is also possible to preserve the original datums and create copies for use as ref datums.
David Janes
Reply to
David Janes

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