Creating Thread Dimensions

This task will show you how to create thread dimensions.
Open the thread.CATDrawing document.
 

  1. Click Thread Dimension in the Dimensioning toolbar (Dimensions sub-toolbar).

  2. In the front view, select the thread to be dimensioned. The Tools Palette is displayed, to let you select the dimension representation.

    In this case click on the thread diameter, and the dimension is created.

    Depending on whether the thread has been automatically or manually created and/or standard has been specified in your 3D document, you will have following cases:
     

    Automatically created 3D Thread without a standard Automatically created 3D Thread with a standard Created 2D Thread with no association to 3D Thread
         

    • The dimension is created from a 3D thread and this 3D thread has no standard.

    • The dimension is created from a 3D thread and this 3D thread has a standard.

    • The dimension is created from a 2D thread (no 3D thread is associated to this 2D thread) or from two parallel lines.

    • The value of the thread diameter dimension will be the 3D thread diameter value and a diameter symbol will be set as a prefix on the dimension. This prefix can be edited and will be not deleted or replaced at dimension update.

    • The value of the thread diameter dimension will be the description of this 3D thread (the prefix of the dimension cannot be defined).

    • The value of the thread dimension is the diameter of the 2D thread (top view) or the distance between the lines (side view) and a prefix M is added to dimension value.

    • The thread diameter will appear as:
       

    • The thread diameter will appear as:
       

    • The thread diameter will appear as:
       


    On selecting Force Horizontal Dimension in View the dimension would appear as:  Dimension1.object > Dimension Representation > Force Horizontal Dimension in View



    (or Force Vertical Dimension in View).

  3. Click Thread Dimension again.

  4. In the section view B-B, select just one of the two lines representing the thread to be dimensioned.
     

    Two thread dimensions appear, representing the thread diameter as well as the thread depth.

  • The dimensions are created as feature dimension. If the Activate analysis display mode check box is selected in Tools > Options > Mechanical Design > Drafting > Dimension tab, these dimensions are therefore displayed using the color defined for Technological feature dimensions in the Types and colors dialog box (click the Types and colors... button in the Analysis Display Mode area).

  • In top views, you can modify the orientation of threads dimensions.

  • If the thread diameter dimension is created from a 3D thread and this 3D thread has a standard, the value of dimension will be the description of this 3D thread and the prefix of the dimension cannot be defined.
     

  • If the thread diameter dimension is created from a 3D thread and this 3D thread has a no standard, the value dimension will be the 3D thread diameter value and a diameter symbol will be set as a prefix on the dimension. In this case this prefix can be edited.
     

  • If the 3D thread has a standard description, the value of the associated thread diameter dimension is always the Thread Description (Hole Definition dialog box, Thread Definition field) as of the 3D thread. The dimension value cannot display the diameter of the 3D thread in side as in top view (except if you add a fake value).

  • Thread dimensions created on top views are technological features now, so they cannot be re-routed.

  • Thread dimension on top view will stay associative to 3D thread even though 2D thread is deleted.
Be aware that clearing the Thread check box in the Properties dialog box (available via Edit > Properties) will make the thread dimension lose its associativity. It will appear as being not up-to-date using the color defined for Not up-to-date dimensions in the Types and colors dialog box) Subsequently re-selecting the Thread option from the Properties dialog box will not make the thread dimension associative again and it will still appear as being not up-to-date. You will need to re-create the dimension.
 

Thread dimensions based on top views

    
Thread dimensions properties based on top views can be created either automatically or manually depending on whether a thread dimension and/or a standard have been specified in your 3D document. Refer to Creating Threaded Holes to know more about specifying threads in 3D holes.

The following table summarizes information about thread dimensions computing based on top views:
 

No thread in the 3D Document
A Standard Thread type has been defined in 3D document - The thread dimension has been created interactively from a 2D thread which does not point a 3D thread
Dimension creation
  • The Dimension value is set according to the diameter of the 2D thread.
  • The key M is set as a prefix on the dimension.
Dimension update behavior
  • Only the dimension value is updated.
Modification of dimension properties
  • All dimension modifications are kept.
  • The M prefix can be removed or replaced by an other.
Standard Thread type defined in 3D Document
A Standard Thread type has been defined in 3D document - The Thread option is checked so a 2D thread is automatically generated or has been created from a 2D thread which points a 3D thread
Dimension creation
  • The Dimension value is the description of the 3D thread. .
Dimension update behavior
  • If the 3D standard has been changed, this change is taken into account when updating the dimension.
  • If the 3D standard is removed, the value of the dimension is the thread diameter and a diameter prefix is added.
Modification of dimension properties
  • All dimension modifications are kept when the 3D dimensions are updated.
Standard Thread type Not defined in 3D Document
A Standard Thread type has not been defined in 3D document - The Thread option is checked so a 2D thread is automatically generated or has been created from a 2D thread which points a 3D thread
Dimension creation
  • The Dimension value is set according to 3D diameter.
  • The diameter symbol is set as a prefix on the dimension.
Dimension update behavior
  • Only the dimension value will be updated.
  • If a 3D standard is added to the 3D thread, the value of the dimension is the thread description.
Modification of dimension properties
  • All dimension modifications are kept when updating the dimension.
If there is no Thread option checked in 3D a 2D thread can be added manually. The thread dimension is not directly linked to the 3D.
 

Thread dimensions based on side views

   
Thread dimensions properties based on side views can be created either automatically or manually depending on whether a thread dimension and/or a standard have been specified in your 3D document. Refer to Creating Threaded Holes to know more about specifying threads in 3D holes.

The following table summarizes information about thread dimensions computing based on side views:

No thread in the 3D Document
A Standard Thread type has been defined in 3D document - The thread dimension has been created interactively from a 2D thread which does not point a 3D thread
Dimension creation
  • The Dimension value is set according to distance between the lines
  • The key M is set as a prefix on the dimension
Dimension update behavior
  • Only the dimension value is updated.
Modification of dimension properties
  • All dimension modifications are kept.
  • The M prefix can be removed or replaced by an other.
Standard Thread type defined in 3D Document
A Standard Thread type has been defined in 3D document - The Thread option is checked so a 2D thread is automatically generated or has been created from a 2D thread which points a 3D thread
Dimension creation
  • The Dimension value is the description of the 3D thread. .
Dimension update behavior
  • If the 3D standard has been changed, this change is taken into account when updating the dimension.
  • If the 3D standard is removed, the value of the dimension is the thread diameter and a diameter prefix is added.
Modification of dimension properties
  • All dimension modifications are kept when the 3D dimensions are updated.
Standard Thread type Not defined in 3D Document
A Standard Thread type has not been defined in 3D document - The Thread option is checked so a 2D thread is automatically generated or has been created from a 2D thread which points a 3D thread
Dimension creation
  • The Dimension value is set according to 3D diameter.
  • The diameter symbol is set as a prefix on the dimension.
Dimension update behavior
  • Only the dimension value will be updated.
  • If a 3D standard is added to the 3D thread, the value of the dimension is the thread description.
Modification of dimension properties
  • All dimension modifications are kept when updating the dimension.
  • In pre-R18 during the creation of thread dimensions, NO-DESC_IN_DRAFTING AND DESC_IN_DRAFTING keys defined in 3D standards determine the dimension type created.
  • There is no change of behavior when updating pre-R18 thread dimensions.   
   
 

Threaded hole dimensions behavior with Standard specified  
  When the standard is specified
Top View behavior Side View behavior
   
 

Threaded hole dimensions behavior with No Standard specified  
  When no standard is specified
Top View behavior Side View behavior