I have a top-down part that somehow apparently lost its link to the base part (the part that I initially inserted that forms the foundation of the part under discussion here).
Is there a way to repair this link? The base part is still named the same, still resides in the same location, and there are two other parts that also reference it that are doing fine.
I've tried everything, including the "References" button in the "Open" dialogue.
As always, thanks fore any help.
Hi Michael,
The symbol > x means that the in context relations have been broken. Once the references are broken there is no automatic functionality within SOLIDWORKS to automatically repair these.
To see the references that were broken, right click the feature and select List external references, and tick the box "List broken references".
Hope this helps
Many thanks
Adam
Try to open the part 8546-01... (reference part) first then 8546-01a....
It helps SW to repair broken references.
Looks like the reference is definitely broken:
I tried opening the referenced part first, that did not work. Is there a way to manually re-establish the reference? FWIW, I also set to "Load referenced documents:" to "All".
Hi Michael,
Currently as I am aware there is no way to restore that link. Once Broken in SOLIDWORKS the process is irreversible.
Zip your parts and make available for download.
There is a good chance that somebody figured out how to deal with it.
Hi Michael,
There is one thing i can think of but not sure how successful this would be. (Will depend on features following the inserted part and their parent child relations)
1. re-insert the part in question
2. Reorder the inserted part to the top of the tree.
3. Use the roll back bar to under the first feature below the inserted part
4. Edit the feature/sketch and remove the link to old part and re-attach to the new part.
5. Follow this process feature by feature
Hopefully this will work however i am not 100% sure unless i have access to the part.
As Vladimir has said above if you zip your files I am happy to take a look and try, but i can make no promises.
Thanks
I have attached the files as per request.
Thanks for all the help with this!
By the way, as you will see when you open the files, if I were to have to re-model the broken "a" part, it wouldn't be the end of the world as it's a relatively simple part. The idea here is for me to learn how to fix broken externals for potential future situations where it may be a lot more serious.
Thanks again.
-Mike
Hi Adam,
I actually thought of doing that. What I'm not sure how do do is break the link from a feature and then link it to the newly inserted base part...
You can if you know where the original references are, you'll just need to reconnect them.
Edit the sketch plane and select a new one and edit the sketch and reestablish those references by adding dimensions etc...
HI Michael,
So I've had a go at re attaching the new model via updating the references. Not going to lie this is not a quick process for even a simple model like this one.
The process for this was i added the part back in. Added the part in just below the old one the went back feature by feature -
1. Editing Sketch plane and replacing selection to the new part.
2. Editing the sketch and using delete/ display relations to delete all. (I've left all these sketches under defined to save time but theoretically you could go back and use the fully define sketch tool to re define the sketches in exactly the same position)
3. Editing the feature - first using the feature scope remove the current part and select the new inserted part
4. Update and remove/Change and references to old part i.e. up to surface selection.
5. The last bit with the sheet metal I could not get to work without error so i would just suggest recreating these features and would be much quicker and straight forward.
Tip - Make sure at every step you are making sure that the old part has no more reference to the feature you are editing using the Dynamic reference visualization. (Coloured ours that appear in feature tree when hovering mouse over feature)
.
In the attached part i have only suppressed the part for now but you should be able to delete as well (Just left for reference)
Hope that helps
Adam
So I have wasted HOURS searching through this and other Solidworks forums. I see that other people have issues with derived parts randomly losing their reference to the original base part. I also see that this is irreparable in Solidworks. That is fantastic. I now have an assembly where the three main parts are derived from a single solid...two of them continue to faithfully maintain their references...one is destroyed. The intent is to be able to make adjustments to the top level model and have those changes propagate through the other parts that interface at complex boundaries. It is impractical to model them independently so this functionality would be HUGE for product design. Unfortunately, this feature works just enough to fool you into wasting your time building an entire model that becomes USELESS after three months of work. I see Adam Humphries is in the same boat; wasted countless hours of his time because this software cannot execute it's functionality reliably. I hope you were able to use the model that Solidworks destroyed to repeat your work and get back to square one after wasting hours and hours repeating your work. I also hope you can recall what you were trying to do with the model after the software totally failed you and your company/client. I know my client is not happy right now. I should have been able to render a file in about 1 minute. Now, a week later, I may manage to keep my job if I haven't already been replaced by someone using OnShape.
Thanks, Solidworks for reminding me that I made the wrong decision in purchasing this software. BTW, the website says copyright 2014 Dassault...it is almost 2017 and your software still have the same bugs as it did in 2009.
This does not work. Additionally, the time and effort required to go back through each reference feature and sketch reference is tedius and prone to make a mistake. You are better off creating the part again and rebuilding it side by side with the failed part. The chance that the original part may drag the problem with it is what tips the scales against doing this. Why not start fresh?
Go to SolidWorks MakroMania - Tauschb rse (4) Item 35 or standalone SolidWorks Programme - Referenzen gerade biegen
It will allow you to replace missing references via API. Not sure if it works with broken references, but definitely with lost references.
Maybe you can replace the old inserted part with a dummy one and then relink it to the proper one...just an idea.
Broken references, virtual components, derived components, equations, etc... have caused many of us to grow up being bald.. Yeah the software may have a lot of issues, unfortunately there are millions of users that are trying stuff that the software isn't totally designed for using hardware that don't meet specs and to top that off there are poor design practices and poor file management. I've been there and done that, no better then anyone else, still make mistakes, however it also taught me to go back and use what works and what works well, consistently, forget the new fangled features till they're bug free.
Create a stable workflow and make designing fun again, there is no better feeling then being able to open an old model and things are stable, no bloody feature tree.
No you didn't buy the wrong software and I don't think Onshape is going to be what it's cracked up to be, just look what happened over the last week, thousands of people not being able to access their models on the East Coast, connection issues..
Don't forget I remember the frustrations as well.......
The only time you will see this is if you right click and break all external references. As it happens it's a very useful feature in certain situations.
So it's pretty simple don't use the function unless you need it - it does warn you. It's not doing anything it shouldn't do.
In 16+ years of using solidworks I have never seen solidworks initiate this function by itself I would tend towards you have accidentally done it without knowing the full outcome.
Richard;
With all due respect, THIS IS NOT WHAT HAS HAPPENED. I will implore others who read this thread to stop positing ad hominem attacks and blaming users for this problem. I have been using Solidworks for almost 16 years now. I am fully aware of how to (and how not to) break references. If this is what happened in the software, then that is the bug we are discussing. This was NOT user prompted. This has happened to me twice now and I am at a phase in the project where no references have been broken for any reason. Thanks for your input. Next time, please wait until you have a technical response rather than blaming the user for stupidity or ignorance which is essentially what your comment amounts to.
Not to add to the ad hominem attacks - and as long time user myself, I never got in to work and had that happen that I know of, if SW is doing this inadvertently in your situation, did you contact your VAR??
I will also count myself in on this, most (which means a lot), most issues are user mistakes, (not all), I know because I've done it and I've had to go and clean up after people.
Shane sorry you feel offend if you feel this is a bug please report it. Is it possible that anyone else is using the assemblies?
Regardless of that you aren't going to be fixing the problem - once broken they are broken. Hence why you need to report the behaviour.
I plan to do that. I am not offended. I am just getting tired of hearing that I must have done something wrong. When I report bugs, I rarely if ever hear back from Solidworks. These parts are on my local drive and I am the only person with access to the machine. I am a consultant working out of a home office...nobody else could do anything to these files. I am not using PDM or sharing the files in any way. I have a remote PDM vault set up but I am not saving to it currently because of traffic issues (slow) negotiating the server.
If anyone has ideas as to how the references could be unwittingly broken, I would certainly like to hear them. A pitfall like that needs to be identified. Minimally, the company should make it VERY OBVIOUS when this is happening. I know anytime I navigate to a selection or dialog box when breaking references is an option, I am always warned that this is an irreparable action. If there are instances where the user would not be warned before doing this or after, please let me know. That may be what has happened in both (or all) of these cases.
I jumped on this post because I was encouraged by the fact that another user had experienced the exact same issue...I know that I am the only one touching these files. I also checked the hard drive to examine when the files were accessed, changed, saved...whatever. If is very frustrating. Had I been putting them in a PDM vault, The problem may be obviated by rolling back. Not everybody can do this. I suspect that the people who actually "suffer" from this issue are the ones who cannot use the "roll back" to get their butt out of the sling. I just wanted to participate in finding a solution as much searching here and elsewhere has yielded nothing substantive.
I apologize for being combative. I just get frustrated when responses to problems are met with blame of the user. It is somewhat constructive to point out that this is a possibility. Again, my apologies for being ungracious.
You're not too combative - it's good to get some attitude some times and here's mine as well..... I know exactly what your experiencing and was caught in the middle of it for quite awhile here, what threw me off with the initial comment was the broken references with the x's - I don't get them, but I do get broken references once in a while, didn't happen for a few months till today.
The problem with this bug if that's what it is, it's never consistent, everything will work perfect till all of a sudden there are broken references again. I have been trying to figure out preventive measures and I would like to feel I got to the bottom of it, but.... till today.
We have a simple shelf unit that was turned into a custom unit and what I do is open the original file and do a pack & go to my desktop, to make sure all links are broken. I pack & go all the parts, drawings and assemblies in the folder, I use the search and replace to give the files a different name. Then I close the original file and open the new pack & go still on my desktop, I make a few changes to see if the sketches are still working etc, once I feel confident that all is well I drop it into our customs folder and work with the file there. Make all necessary changes and additional components, fix the drawings and close the job.
Now almost a month later it hit's the programmers to do list and he brought the drawing pack back and said there's issues with the model, I'm like what'ya mean something wrong with the model, I quickly open it and sure enough the shelf fasteners are all over the place and the feature tree is red, mostly mates, but some hole wizard location points, luckily this is just a very small assembly only 124 components and most of them are simple fasteners. What happened my main Skeleton Sketch Part was fine, it was the shelf components that were built off of the Sketch Part, I had those weird color yellow dots at the corners of my sketches where the missing links were. I re-established the same links I had done before and closed the project, they might reappear but I doubt it for this assembly.
This was going on for a few years here and it is a big issue when you worked on something the entire day and the next day it just blew up, luckily for me out IT guy was watching me one late afternoon and the next morning when I opened the file I showed him what was up, so I was finally vindicated, till then the guy's would look at me really strange and be shaking their heads when the walk away, I would blame it on the server, they said that wouldn't be possible, it's what you're doing.
Most important prevention that I found was is to use the Isolate command, that eliminates picking the wrong face, vertex, part or whatever....
My issues are not reproducible at will, they pop up a few here, just once in a great while but when it happens, it's frustrating as all get out......
This original post is from 2016..... I now have the same problem. It seams Pack and go maybe the original culprit or problem.
Do I really need to access an API utility for a resolve? I would think there is simply a switch to hit to re-link the references.
MP-R2-Base-1-> x (Default) < the model tree shows this for the INSERT PART How can I refresh the link to the reference part?
Since SW uses that NX kernel I wonder how those engineers resolve issues like this?
Bart Brejcha
Not totally sure that it is possible without completely replacing that insert feature.
I completely replaced the 'insert part' feature. Managed all the failures that came. Another question. How can I turn on feature numbers in the model tree. What Im looking for is a second column 'Surface-Offset15' can be hard to locate on the non failed model and it takes time to search which is why I want a second column.
Bart Brejcha
You can rename anything you want in the feature tree.
Also, if you KNOW the name, then use the filter that is already at the top of the tree:
The inserted part is not open in memory. There is a system setting to fix this (not at my computer right now so I cannot look it up). In meantime right click and select edit in context than ctrl tab back to your model.