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Fast Facts! Quick Tips for Using PTC Creo - Drawings Part 2

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Fast Facts! Quick Tips for Using PTC Creo - Drawings Part 2

Today’s “Fast Facts!” post focuses on displaying set datums and erased dimensions and axes. This content is intended to provide users with easy-to-use, actionable tips and tricks for how to use PTC Creo more effectively. These tips come from Steve Meyers and Evan Winter, two PTC Creo experts in our training group.

 

1. Displaying Set Datums on Drawings

Set Datum visibility can be controlled through layers, but they can also be deleted or erased.

 

For example, in this drawing there is a Set Datum that is currently erased and is hidden from view. Although we can select it from the Drawing Tree and “Unerase”, it will still be hidden if it is on a hidden layer.

 

The easiest method of controlling Set Datum display is to:

  1. Leave layers containing Set Datums “shown” in the drawing, or remove the datums from layers if possible.
  2. Delete all unnecessary datums from the drawing views, leaving only the ones desired.
  3. Use the Show Annotations command at any later time to retrieve additional Datums for a particular view.

 

An alternative method for controlling Set Datum display is by using view-based layer status (Explained below).

Picture 1.png

2. Displaying Set Datums on Drawings (Alternate Method)

Drawing views can have their layer status set independently of the top level drawing.

 

To set the layer status for an individual view:

  1. Pick the view from the layer tree Active View drop-down.
  2. Set the layer status to enable the layers for this view to behave independently of the drawings layer status and be managed separately. In this example, we would Unhide the layer containing Set Datums.
  3. Return to the drawing (TOP MODEL) in the Active View list and Hide the layer containing Set Datums. The layer is now only shown in the single view.

 

To restore the layer status of the view back to that of the drawing:

  1. Select the view again in the Active View list.
  2. Click “Drawing Dependent” in the Layers drop-down.
Picture 2.png

3. Dealing with Erased Dimensions and Axes

Some WF4 drawings may have a large number of erased items that must be deleted prior to being shown in a different view. These can be deleted automatically through a hidden drawing option.

 

  1. Using the File menu, select Prepare, then Drawing Properties, and finally Detail Options.
  2. To delete erased dimensions enter user_command in the Options box and delete_erased_dimensions in the Value box.
  3. Click Add/Change.
  4. To delete erased axes enter user_command in the Options box and delete_erased_axes in the Value box. Click Add/Change.
  5. To apply the user commands, click Apply or OK. The user_command is applied once and is not maintained in the .dtl file. It can be run again later if required.
Picture 3.png

 

Stayed tuned as we cover more PTC Creo commands, features, and shortcuts designed to help you use the product faster!

 

For more in-depth product feature explanations, visit our Tech Tips area.

 

Have some ideas about what you’d like to learn more about? Send me a message or leave a comment below and we’ll write up the best ideas from the community. Thanks for reading, looking forward to all of your feedback!

1 REPLY 1

Re: Fast Facts! Quick Tips for Using PTC Creo - Drawings Part 2

Works great until someone sets a datum or adds an item with a set datum to a subassembly and then -those- datums need to be dealt with. Again.

Typically the newly 'set' datum will be on a newly created layer, so that new layer will automatically be visible on the drawing and with it the shown datum.