Showing Theoretical Bend Intersections on a Drawing
Click File > Prepare > Drawing Properties. The Model Properties dialog box opens. Click change in the Detail Options dialog box. The Options dialog box opens. Set the following options to control the display of theoretical intersections and bends for bent tubes in a drawing:
• show_pipe_theor_cl_pts controls the centerlines and intersection points:
◦ To show centerlines with bends only, specify the value as bend_cl (the default).
◦ To show only centerlines with theoretical bend intersection points, specify the value as theor_cl.
◦ To show both bends and theoretical intersection points, specify the value as both.
• pipe_pt_shape controls the display of the intersection points. To specify the display, set it to cross (the default), dot, circle, triangle, or square.
• pipe_pt_size controls the size of the intersection points. To change the size, modify the numerical value.
When you change the setting of any of these options in the drawing setup file, Creo Parametric updates all centerline and point intersection displays in the drawing, but you must repaint or regenerate the view to update the views.
If you create a dimension to an intersection point and then change the setup options to turn off their display, the dimension remains and is associative.
To control the hidden line display of the pipe centerline in drawings, set the drawing setup file option hlr_for_pipe_solid_cl.
To update pipelines created in previous releases, set configuration file option pipe_update_pre_20_int_pts= yes to get intersection points entities. These entities are created in session when you regenerate the model or when the model is retrieved.