Cordell Hollingsworth

Workaround for how to suppress a line as part of a weldement profile sketch

Discussion created by Cordell Hollingsworth on Jul 25, 2014
Latest reply on Jul 25, 2014 by Cordell Hollingsworth

I have finally figured out a workaround for how to suppress a sketch entity such as a line in a Solidworks sketch.


Here's how I did it for multiple lines in my configurable weldement profile.  By the way, you’ll need SW2014 to add configurations to a weldement profile like I did.


intended line: the line we are trying to toggle between "solid" and "for construction"

parent line: a line that we will copy to make the sketch appear to work intended

hiding spot line: we will hide the "parent line" in this line

2nd line: an extraneous line in our pattern

3rd line: a solid line that we toggle on and off using configs



  1. 1. Toggle your "intended line" to "for construction".
  2. 2. Identify a line parallel to and of greater length than your "intended line", this is your "hiding spot line".
  3. 3. Divide the "hiding spot line" into two segments. One of these lines will be your "parent line".  Do not add any relations to define the length of the "parent line".
  4. 4. Create a linear pattern of your "parent line" and set the instances to 3. We need to use 3 instances because Solidworks requires a minimum of 2 instances for a linear pattern.  Make sure not to add any relations defining the position of the pattern.
  5. 5. Toggle the second line in your linear pattern to “for construction”. We won’t touch this line again.
  6. 6. Drag the third line in your linear pattern over your “intended line” and let Solidworks attempt to add relations.  Hopefully this merges the end points of your third line and fully defines your sketch.  At this point you should be able to exit the sketch and build your custom profile using weldements.  Make sure your document builds correctly before continuing.
  7. 7. Create a new configuration of your sketch. In this configuration change the instances of your pattern to 2.  This will delete the third line in your pattern effectively toggling the your “intended line” between “solid” and “for construction”.  This may delete the relations that you added in your first configuration so you may need to go back and add those again.  In fact any time you make changes to your second configuration you’ll need to make this repair.  So make as few changes as possible once you’ve decided to try my method.


Later steps:


You can combine the steps I mentioned above with other sketch operations to configure sketch geometry in ways that you were never intended to be able to do.  For example, by combining my discovery with a mirror operation I was able to merge and unmerge edges of my T-slot profile in different configurations of my profile.  This way I can have all of my T-Slot profiles driven by one configurable weldement profile instead of 50 different files.  To this effect I can change the profiles of my weldements and not have to redo mates if I’m working with them of the assembly level.

Capture profile.PNG

The "hiding spot line" is highlighted in yellow, the "parent line" is covered in red, and the "3rd line" and the "intended line" are overlapping, I marked them with blue. The dotted line in the middle is our extraneous "2nd line".

Capture profile 2.PNG

In the new configuration the "3rd line" disappears but the intended line remains (circled in blue).  I also configured the "intended line" to change length and move to the axis of symetry that the lines are mirrored about. This causes the endpoints to merge and the profile to rebuild as intended.

Capture45 45.PNGCapture45 45 3S.PNGCapture 45 45 2SA.PNG

Each of these profiles uses a different configuration of my custom weldement profile.  The faces merge without creating unwanted seams.  The mates seem to be rebuilding as well.