I slid something up and back down the feature tree, and now all my in-context references are broken. Can I fix offset entity errors like this? I haven't found the magic drop down/radio button/ check box, tab, whatever to do this.
I wish I had an answer for you, other than "no". I am responding just so I will know if/when someone gives you a better answer.
if you haven't saved the model after the move, I either exit SW without saving and then re open the part and all should be good again, and don't do that again
the items you moved which helped define this item must exist prior to making these, since you moved them they no longer exist prior to this feature.
If you can move this part of your part along with what you moved previously then you could avoid the issue otherwise it appears you would need to delete the dangling relationships and redefine the entities. If you can close out and restart and then make the move to include this part you may be able to correct your issue.
Personally I have found in many cases staying in context is difficult in large assemblies in most of my work which is Die Design mainly. It seems awesome to keep everything related and be able to change one dimension and it change everything related, but keeping all of those relationships is difficult.
You put in a relationship to an edge and then later you put a chamfer or radius on that edge and the relationship is broken. Some choose to just design sharp cornered and expect Die Makers to put all the proper corner releifs in, but in some cases if you do that and they dont you have failures. Same thing will get you if you put in a smaller cham/radius and go larger later.
I'm not running SW2014, but it looks like you are. You might want to look into the Replace Entity feature. (That might not be the right name.) I'm not sure if it will work for an offset, but if it can, then that should make life much easier. If it doesn't, then I think the bad news is that you will need to delete your Offset Entities and redo them.
That is probably the best you can do. I'm not sure how well it will work, and it will be somewhat time consuming, depending on how many edges need to be replaced. Hopefully it will save any of the downstream references. It is probably as good as it gets in SW. Even if you picked some edge and then told it to offset the chain, I think it still treats all those edges as individual references. Not like you can replace the whole chain by just selecting a single edge. Kind of hard to explain. The 2 ways to think about it are: 1. a bunch of individual references 2. a single reference and everything connected to it.
While you are doing this, you might want to start by offsetting the sketch entities by 1/2 or maybe 2X what you want in the end, and then once you have done the replace you can change the dimension to the value you really want. This will just keep things from being on top of each other while you do the replace.
Fortunately it was a simple drill fixture, and I just remade it. I also noticed that I lost relationships when I changed the (fixed) enclosure that I made the fixture from to a virtual part. I'm not sure why, but I'll guess that you need to start with a virtual part. At any rate, it's done, and it's good.
Nice using REN Shape I see
Is REN shape modeling board? I made the drill fixture using a Makerbot Replicator2X 3D printer, & slate gray ABS filament.
REN Shape parts
OK, kind of like Garolite, but maybe without the weaving.
No way to fix it , would be nice we there was... seeing as most of us have been in this situation before.
Yeah, like Lenny said, the easiest way to undo it is to use "Reload" (but you'll lose all the other changes you've made). Perhaps test this with a parallel save-as-copy first - it might let you then copy and paste the new features into the reloaded part.
Otherwise you have to manually recreate the offset relation (add linked dimensions between each set of lines or use equal construction lines to define that distance).
Chris's answer reminded me of another workaround. If your offsets are all lines and arcs, then you can remove the offset relation and then add the relations that you need such as tangencies, concentricity, equal radius, etc. When you have it all nicely defined you can add in a dimension for the offset and it all becomes nicely editable. If you've got splines, you are typically screwed.
I've done that before when I've seen broken relations, or just didn't want the part tied to the model anymore. Actually, I prefer to remove external relations if I can.
External references can be troublesome, I can see using them for items were projected changes are minimal, but if you are certain changes are common, it is best to stick to old school brain power and dimension/relate internally.
Using blocks for sketchs can be a good way for multi-use of common features and help prevent external references but yet use those already defined features.
I once had a gussetting feature I intended to use in several places, I defined the first sketch as a block and then inserted that block for the following gussetts. In the end I had to alter the original gussett as it cause an issue, I was able to change it without causing issues with the others due to the block use.
One of the few consistant things in life is "Change", planning for change isn't easy but can save a great deal of pain in the end.
*This actually did not work on this particular scenario. Back to the drawing board... If the end point of the offset dimension could have been moved, it would have worked just fine.
If you can recreate new geometry to base the offset off of, or lets say like in my case I added a chamfer then the following would work.
Edit the sketch that you used to create the offset.
Right click on the dimension for the offset and select "Display/Delete Relations".
Select "Dangling" from the relations drop down.
Select each item, and select a new correct edge for the offset of each sketch entity.
Then click the replace button at the bottom of the entities section.
Click the check, and Bob's your uncle.
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