Losing references

joseph_newcomer

I just got a message that a sketch failed to regenerate.  When I opened it, I got the message "Some external references are missing".  Unlike some systems I have used, this one highlights the failure point; apparently the coincident constraint I had used to create the rectangle disappeared when I filleted the wall shown, which is the rear wall.  Why does a fillet make the abstract wall border disappear?  Also, as I have observed in an earlier post, this causes the two walls to fillet independently, when I want them to fillet as if they are a single wall.  What I need to do is, without bizarre construction of walls, to create four independent walls around something that act as a single wall.  But I need to have a way to reference an unfilleted surface and not lose that reference when I fillet it.

NeilCooke

Add the fillet after the sketch.

chandra_harsha

So, if the fillet radii on both vertical edges, make the corresponding face move away from its original position, then any sketch entity that has reference to this face will go into error.

"corresponding face move away from its original position" - What I mean by here is. Lets say you have a face of width 25mm, at the corners when a fillet radii is less than 12.5mm, you still have this face present. But once fillet radii crosses or equals 12.5mm, the face will disappear, and cylindrical face will start to appear. Any fillet radii above 12.5mm, this cylindrical face will start to move inside. 

So, from the picture you posted, I think this is the issue that happened.

I didn't completely understand your single wall question though. 

joseph_newcomer

The problem is that I have an "abstract image" of something, say a rectangular channel.  I do it by creating a rectangle on one edge and doing a "remove" extrusion to the opposite face.  Great.  Now, I want to use the parameters of this rectangle by doing a "use" into another sketch.  Great.  Now I want to fillet the corners of the original channel.  I would think that the rectangle I used would remain intact, unmodified by the fillet.  But no, the original sketch is discarded and replaced by a new sketch which is based on the result of the fillet.  I solved this by putting the rectangle on the opposite side of the object, and doing a "use" into the side I want the channel it, and the other part which did the "use".  This is remarkably ugly.  Putting a fillet into an extrusion should not alter the underlying sketch that defined  the unfilleted extrusion.  I also tried to put a point in that was made coincident to the horizontal and vertical lines, so in the part drawing, there is a point visible.  But when I go to the assembly, I can no longer find that point, which, unfortunately, is what I need to use to establish the sliding point for the two parts (they have to be .2mm apart, to allow for the Teflon tape that will be put in the final construction.  The fillet is incidental, and might change its dimension, but the reference point will not change, nor will the point on the object that is doing the sliding.  In other words, once I establish the relationship of the lower-left corner of the unfilleted object with the lower-left corner of the unfilleted channel it is sliding in, any filleting should not change these reference points.  Consider the filleting "decorative" (well, it is to reduce stress points, but from the logical viewpoint of my device, the fillets are "decorations").  So the problem boils down to how do I create a fixed reference point?

An example can be found at
https://cad.onshape.com/documents/0629d23252e89bb200a38cdb/w/f085a508111c63168ed8dc57/e/caf9c0d967791f7c365288ea?bomType=flattened&renderMode=0&rightPanel=BOMPanel&uiState=61f37fdbeab11f5866bd41c4

Note that I have created two mate references in the assembly.  What is annoying is that I can't use #tape_thickness as my offset when I create the mate; I have to know what it is and type in a number.  This violates abstraction.  Now, at some point, I may want to fillet the channel or the slider.  Nothing else should change.  My reference points need to be based on the abstract original geometry, and the fillets are irrelevant to the proper maintenance of the relationship of the two parts.  I also need to reference the #tape_thickness in the assembly.  I should be able to change #tape_thickness or the fillet radii at any point without causing any disturbance of the assembly, in particular, the slider mate should always continue to work.  I don't mind if I have to do something extra to make this work, hence my attempt to create a separate point unrelated to the filleting.

alnis

@joseph_newcomer for that bar in a slot, here's a way you can keep the feature tree clean, simple, and robust by using some unique features in Onshape (use mate connectors to keep mate references stable, use "master sketches" that produce multiple parts, take advantage of how you can relate designs in multi-part part studios):
https://cad.onshape.com/documents/3e781a2548a5ade8a92bdac8/w/1f317ad4cfe4feaf7048beb3/e/22507e9c7d7365e6689093f4