CREATING DATUM CALLOUT IN DRAFTING 1

[kadego]

Hi Group
Can someone please explain how one creates a datum callout?
CATIA V5 has a dedicated icon which creates it in one step.
I know NX-3 has an equivalent function but how?
Thanks
Dave

 

[zora65]

Kadego,
In drafting, open the annotation editor and make sure the GDT symbols tab is selected. Along the bottom row you'll see datum letters A through F. Select the needed letter, choose the placement leader type from Annotation Placement window and place the datum. Hope this helps.

Bsilk
Senior Designer

 

[mjcole]

I have used the following to make placement of the datum symbols easier to move similar to Pro/E which allows you to put the datum symbol [COLOR=white black] A [/color] on the opposite side of a dimension or with an extension line to a datum surface.

Switching sides
Use Edit Object associativity to switch extension lines.
Move ExtLine1 to another entity.
Move ExtLine2 to the former ExtLine1 one reference.
Move ExtLine1 reference to the former ExtLine2 reference.

Movable Datum tied to Extension Line
Create a Horiz or Vertical or other dim with extension line 1 referencing your datum surface.
During creation of the Dim select the Annotation preferences A icon and on the dimension Tab select both arrows and the second leader to be toggled off.
Use the Automatic Placement as dimension type.
After creating this dim you can use the edit annotation icon and replace the dim value with a space.
When placing the Datum Symbol [&70]<+>A<+>[&90] use the Datum leader type and select the Attached to Dimension placement type.
Select the Manual Dim with the datum extension line and then pick where you want the center of the Datum Letter to show.
The placement must be on the opposite side of the extension from the Dim Text location or your leader will be placed at the Drawing origin.

Hope this helps other people like me who work without the GD&T application license.

Michael