Dear Sir / Madam,

I'm not a real CAD engineer (I am actually a system architect), but use SolidWorks to validate some concepts / principles. Now I have a rather elementary problem, for which I would like to ask your help:

I have a problem regarding a relationship between two dimensions in a sketch, which I want to dynamically update in a pattern feature, see the attached model. Here, I have sketched a fiber with diameter 0.145mm, where the horizontal and vertical "radius" is equal to 15.350 mm from the origin (so this is the 1: 1 radius). Now, I would like to create a pattern of this "bent fiber" with a pitch in X of 0.25mm, where the Y position will shift 0.17mm. In order to realize this, I already have drawn the fiber as quarter elipse, where the y-radius is made dependent on the x-radius.

See "sketch 1" in this model attached ("first fiber"), the above idea works (vary the horizontal dimension to a value > 15.350 mm, then it runs nicely along the vertical proportional to the 0.25/0.17 ratio, also see model "last fiber"). Then the following steps seemed simple to me: just make a sweep, and then "pattern" in x-direction and "vary sketch" so that the y-dimension is changed dynamically during the pattern formation. Unfortunately, this does not work, the vertical size remains at the initial starting height of 15.350 mm and does not increase according to the relation I have put in the sketcher

From my past, I am quite experienced in the application Pro/ENGINEER (Wildfire, all possible courses done) where the below issue was easy to solve this problem with the above method. Unfortunately for SolidWorks this method does not work. Any suggestions to make this work easily in Solid Works?

Thanks for your efforts!!!

Roy.

This issue came up in another discussion recently, I think SW fails to update equation results for each instance when "vary sketch" is used. The best way to make "vary sketch" work is to have all sketch relationships be done with relations. You sort of need to get creative to convert an equation into sketch relations, one method is to use construction lines. See my attached example where I established the same x and y relationship with construction geometry. Note that your equation can be reduced to y = 4.912 + x * (17 / 25).

Also, I believe that "Vary sketch" only works for feature patterns, and feature patterns only work if all instances can result in a single solid body. So another alteration I did was to extrude a block that each fiber would touch so the whole part after the pattern is one body. Then after the pattern I cut that block away.