How to Fix Broken External References

Helepolis,

What do you mean by formatting your computer? Did you reformat the hard drive? Did you change filenames or file paths?

Examine your part files and see what assembly they are attached to.

--
JHG

This is why I don't do top down, especially with master sketches.
You will have to go thru each part and fix each reference to the master sketch. A long and tedious process.

Chris, CSWP
SolidWorks
ctophers home

Hi, Helepolis:

Reformatting your C:\ drive should not cause your issues. Your assembly and sub-assembly models should rebuild properly as long as you have all the files you need.

If you lose some of the files, you can fix them manually. It needs a lot of advanced skills to do it.

Best regards,

Alex

Hi, Helepolis:

You will have to pinpoint the area that causes the issues. Did you inadvertently rename one of the files?

Best regards,

Alex

External References... sigh.... I do a lot of top down design. If I have to keep the top down design I use the Freeze bar. Anytime I can remove the references I do because some times those references becomes lost. Its as easy as an the ID of a line changes or a single mate flips on you and then the whole assembly is trashed. You have to have some advanced skills to find what is causing this to occur. I have wasted an entire day trying to find the culprit and I have been using SW since 1995.

My first suggestion is to start suppressing parts\sub-assemblies and see what happens it might get better, or it might get worse, but eventually you should get to a point to where its helping you narrow down which file or files that might be having an issue. Like I mentioned above it sounds like the in-contexted reference has become lost. The only way to fix it is to find it and repair it.

If you have not been doing you this need to start using it often and that is Ctrl-Q and I do it couple of times to make sure everything updates. If you have a large assembly its possible you might have circular references and that one could be hard to find. That is one reason why I rarely and never recommend using "Allow multiple context for parts when editing in assembly" without having a good understanding of Top down design along with the does and don'ts.

One other thing I don't know how you in-contexted your files in the assembly and maybe this will not help, but many moons ago when I was learning about top down design. I used planes in my assemblies to control my sketches in my parts, and used plane to plane mates in my subs, versus other geometry from other parts etc. Then I controlled those planes in a Design table, and used equations inside of the Design table to control the assembly. Made it much easier to handle and for other people to use. Of course it was on server. I hate the Cloud for any type of SW file sharing especially accessing and active file. Files need to be local and not shared over a network... That could be part of your problem. Maybe the format changed a drive letter to an external location. Another reason to use a server or PDM. You can use a UNC path versus a drive letter. Drive letters can change. UNC path is a direct path to the server file location. You don't get that option with Cloud storage. I don't know if this is true or not, but you might check with IT and see if there was a cookie or something that you previously had that was removed during the format which is causing this to occur. That sounds to me like it would be the same as drive letter change.

Top down is great for making things update automatically, and giving you automation, but its a freaking nightmare when this happens. Sometimes its easier to break all the links in the files, and rebuild the assembly and re-incontext all the files. Depends on how much time you can devote to finding the problem(s).

I hope some of this helps you find an answer.


Scott Baugh, CSWP
Mechanical Engineer
Ciholas

"If it's not broke, Don't fix it!"

Click to expand...

faq731-376

Hi, Helepolis:

Solidworks assembly file (top level) is like a branch of trees. You can send this branch to anywhere in the world. Anyone who receives it should be able to open it without errors. Solidworks uses relative memory addressing in resolving the assembly. So, it does not matter where the files are located. URL of the files (parts, assemblies, sub-assemblies and drawings) do not affect rebuilding of the assembly.

If the original assembly was successfully rebuilt, the issues must be caused by someone who renamed and/changed some of the files.

Repairing a dangling part or an assembly should be easy as long as you have skills to view relationships between entities. Sometimes, you see a lot of rebuilding errors. But they may be caused by a single error.

Best regards,

Alex

My guess is that you lost your default search locations when IT worked on the computer. If you have references in different locations it'll be a mess until you tell SWX where to look, then it should be fine.

This is useful about where SWX looks for references in what order. You probably lost #2.


You can use the SWX settings wizard to make a file to restore your settings when things hiccup and they are lost.