Have you ever had solidworks refuse to show the sketch as fully defined, even though it is?
Can you toggle sketch relations (ViewâŚHide/ShowâŚSketch Relations) and post a screenshot?
Iâve seen something like this, done as a sketch symetry, happen once in awhile. I believe it has to do with the symetry âplaneâ or one of the geometry lacking a relation that is implied within.
I deleted the two blue lines and redrew them. After that it needed another constraint and was happy. Previously adding a constraint made everything yellow.
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Can you drag the blue line left or right? Without seeing the relations itâs tough to tell, but it looks like you have the 2 outside lines a set distance apart but not set to anything side to side (I would assume a dim from the c-line to one of them half of 1.875 would do it)
The two horizontal lines are equal length.
If you watch the gif, I try dragging both lines and 3 corners.
yea, weird
Iâve had it happen a time or two. I force myself to ignore it and go on with my life, but itâs a struggle.
I tried. I really tried.
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I will have to give that a try next time.
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Word of caution for those that donât know, the sketch lines determine the face IDs that get created. Deleting a sketch entity and redrawing it will dangle any mates and dimensions in assemblies and drawings to those faces.
We train users to avoid deleting sketch geometry if at all possible. Although sometimes you have no choice. In this case, you could try toggling âdetach segment on dragâ, I added to the sketch toolbar, otherwise its buried in the menus. Then reattach and add relations back.
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That wasnât a problem here, but is good advice.
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This has gotten me into trouble a few times till I learned! Now its, âthink twice before deleting a a line segment from a sketch!â
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There are some tricks to keep the mates intact. Hereâs an example. I have an assembly with two of the same part mated concentrically:
The part is made from a revolved profile:
If I delete the top line and redraw it, the concentric mate fails:
However, if I do this:
- Add a sketch point coincident to the line
- Delete the line
- Redraw the line
- Add a coincident relation between the sketch point and new line
then the mate doesnât fail:
I can delete the sketch point as a final step.
The sketch point seems to keep the new sketch entity associated with the faces so they donât get new IDs.
This only works if the new line is the same as the old. Replacing a line with the same line isnât very interesting though.
Rather than delete, the Split Entities tool or Detach Segment on Drag (under Sketch Settings) let you do things like turn the original profile into something like this while keeping mates intact:
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There is also the âReplace Entityâ command introduced a few version back that is suppose to help with this. It does keep the relationships.
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Iâm late to the party here, but if those two vertical lines were just parallel, it wasnât fully defined. Especially if the dimensions to the endpoints were just to endpoints, not to the perpendicular lines on the ends. I know you tried it, but the corners are probably still free to move horizontally. Dimensioning to the center axis (which is an actual axis, not a sketch line, right?) would fix it, or making one of the lines vertical or perpendicular to something. Just a guess.
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One of the subtle, yet significant, differences between SW and SE. Solid Edge didnât merge points. Instead, points could be made coincident with sketch relation, to move them just find and delete the coincident relation. Because of this there was no need for âDetach Segment on Dragâ. Still a minor frustration in SW sketching. A serious blunder for sloppy modelers that delete sketch elements then complain about blown up assemblies.
Iâm pretty sure I tried everything possible. Adding an extra constraint either did nothing or turned a couple of dozen constraints yellow. I wish I had saved it before fixing it the hard way.
In SWX, I did confirm that relation/references to one endpoint is lost when you merge them. I thought maybe it was just putting them on top of each other with a hidden coincident. But no, not sure why this is desirable and seems easy to fix and would go a long way to the perception of stability. Just not flashy enough for the market department though.
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