Does anyone know how to break the "linked to parent part" properties?
I've been using weldments for quite some time and have never seen this.
I had this problem and the way it was fixed was by deleting the properties using the windows explorer.
Right click on the solidworks part file in windows explorer and click on Custom Tab of the file properties.
You will be able to remove the individual properties from the file.
for some odd reason that tab doesn't exist
I never seen this before did you try to reset your system option?
So here's a screenshot of the dialog box that allows you to accept or deny the linked properties.
The funny thing is all 3 parts were created in 2015.
It's related to inserting a part into the weldment.
In this case 2 different flanges.
I've just opened up your parts and inserted another copy of one of the parts. I got the message on inserting. I didn't get the link to parent issue until I added values. The easiest way to get rid of the values is to uncheck the Transfer>Custom properties option on insertion of the part (or go back and edit it).
Someone must have wanted the values to always link to the parent part hence the change. The way to get the values in if you want the fields but need to modify them is the old fashioned cut and paste. I know you have used weldments a lot so I may be telling you something you already know.
I'm using SW2015 SP2.1
Thanks, I went back and reviewed and I didn't have the transfer custom properties checked.
I couldn't get any custom properties to stick.
I created all of these parts in SW2015.
I created the 1.5" flange by using the "Save As" command from the 8" flange.
Because of this behavior it would seem that the 8" flange is the parent.
Not sure why the "Save As" part acted in this manner.
It's almost like the "Save As" command can imbed information into the part.
I've never seen this behavior before.
It would be nice to know how to toggle the "Linked to Parent Part" off and on.
The pop-up message gives you the option to accept or decline but it doesn't work.
But the odd thing is these parts weren't created in a version before 2014
So in that regard I don't fully understand the Yes/No question.
I just created the 1.5" flange from scratch (new) and inserted and have no issues now.
Did you try the "Save As Copy" or just save as??
I'm not getting exactly the same behaviour you describe. I only seem to get the linked properties (shown in the first image) when I tick the insert custom properties. Seems a bit weird, anyway at least you seem to have got it sorted now.
What you describe is one reason I don't often insert a part into a part, I've had so much frustration.
This is the response from my VAR.
""I believe this is a known issue and is related to SPR 798694 “Properties shows 'Linked to parent', even when references are broken, when check Custom properties to transfer to cut list properties for insert part.” I’m able to reproduce the issue you’re seeing though by simply inserting a part into another and linking the customer properties. Once they’re linked, I cannot unlink them. The only way to break the link, that I have found, is to delete the parts and then re-insert them without selecting the option to link the custom properties. Your files did have this option selected but if it was selected when they were initially inserted, then this is where the problem is originating. You can try deleting and reinserting the 1.5 and 8 parts to test this and see if you’re able to modifying the custom properties in 370.7103. I did test this myself and it seems to resolve the issue although you will have to fix broken references. I’ll add you to the SPR but please let me know if you have any further questions or can reproduce the issue using different methods.""
Apparently I selected "Yes" to maintain link but when I tried to unlink I couldn't (bug SPR 798694).
The solution was to delete the inserted parts and re-insert them.
I have a mature assembly with lots of parts created from a parent. This bug has set me back a day now.
I am not sure if all of these steps are required but this seems to be working for me:
I just came across this issue today and have a workaround. Use SolidWorks Explorer:
NOTE: this doesn't remove the "Link to Parent" property in the part itself, it just changes the "Evaluates To" field of the property. This achieves what you may want (I have text fields in drawing documents linked to part file properties, and they updated correctly). But there must be a bug because you are still unable to edit the properties while you are editing the part in Solidworks. You can only ever edit these properties in SW Explorer once they have been linked, even if you break the link to the original part.
Now that I've explained the workaround, I'll explain what brought me to this issue:
I created a master part with multiple solid bodies, and then saved those bodies as separate files with their custom properties linked to the original part. Since "Save Bodies" actually becomes a feature in the Feature Tree of the master part, I tried editing this feature and unchecked "Copy Custom Properties to New Parts." But this doesn't solve the problem because apparently if properties have been linked once, they will remain linked. Even breaking the link to the original part doesn't solve the problem, as you have probably already discovered.
I've been having problems with this as well.
I do a lot of modeling with master parts and then save out bodies. It seems that in the save bodies (or split part) dialog box, solidworks automatically activates the "copy custom properties to new parts" check box whenever you make any changes. You can turn it off, but then if you change the name of one of the parts, the option gets turned back on again automatically. Unchecking that box has to be the last thing you do before ok'ing the dialog box. Once you've saved out the bodies with that option checked, I couldnt figure out any way to fix it (in Solidworks) without deleting the parts and trying again.
This is extremely frustrating, especially since I do a lot of the filleting in the "child" part file to keep the size of the master manageable.
Tried the workaround that you suggested. Seems to work, although it does leave some discrepancies in the custom properties...
A quick work around is to enter your desired properties in the configuration specific properties, as Solidworks will use those before it uses any custom properties of the same name. Works well if you don't have a bunch of configurations already.
Was a quick/easy approach to being able to edit/delete these properties ever found?
I just ran in to the same issue on a bunch of mirrored assemblies with mirrored parts. The parts do not have the issue, however their assemblies do.
If you do not already know this. Issue with greyed out properties ("Linked to parent...") is caused by making derived parts
with custom properties ticked.
You can remove the lock on the proporties by listing external refs ans braking them all.
I wanted to add to this comment. I created a derived part and did not uncheck the custom properties box. I was unable to change the configuration specific properties, even though I ran the gauntlet of all the different fixes listed on this thread (i.e., breaking all external references, re-editing the in-context part, Using SolidWorks Explorer to modify the properties, etc.). In the end everything reverted back to un-editable Linked to parent property. (Please note that these fixes may not have worked due to the early version of SolidWorks 2017 (SP 1) that I am currently running.)
At any rate, I found a new way around this problem. As I was going through the tutorial for SolidWorks Treehouse manager, I noticed that you can directly edit the configuration specific properties of any part.
I went ahead and created a new tree house template from my existing assembly, updated the problematic properties, and then hit the 'export to SolidWorks documents' button to override my existing models.
I then opened up the problematic derived part files. Although it still appears that the configuration specific properties are still linked to the parent part (see image below), these properties are actually overridden via Treehouse manager.
I had the same issue, workaround was to INSERT THE PART AGAIN with linked properties, then delete it. This unlinked all the config-specific properties, though it did not unlink the custom properties.
Update - to unlink remaining custom properties, INSERT THE PART A THIRD TIME with "Break link to the original part" option checked. Then delete it. Delete all the properties as some might be bad. Then re-add.
Thanks Terry, this solution worked for me (SolidWorks 2016).
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