Good day all
I have another problem I am struggling with.
In a draft you usaully get that grey Thick corners when something isn't correct within the Assy or model, well I Have a couple of assemblies where I can not get rid of that Grey corners.
I've tried drawing view tracker, properties update and everything, still nothing happens.
Can someone please help me with this annoying problem?
Thanks in advance.
I would suspect there are broken links, usually from using "Insert Part Copy", where that part has been renamed, or has an altered file directory.....simply re-pointing that to the correct file, should fix this. Sometimes, it can be several part copies deep, and all parent/child relationships need to be satisfied before the grey corners will go away.
One trick, is to place a view of individual parts in draft, and the grey corners will be on those affected parts.
Design Manager Streetscape Ltd
Solid Edge ST10 [MP8] Classic [x3 seats]
Windows 10 - Quadro P2000
Testing: Solid Edge 2019
Sometimes, when you can't find the reason, the reason is a part that's not updated automaticaly.
When you insert part-copy and this part-copy is not updated automaticaly you won't be noticed of this in draft. A real PITA...
So you need to think which part is constructed whit part-copy and open each one to update.
If running ST7 or ST8 and the model inserted into the Draft is an Assembly, open that assembly and use the Component Tracker on the Tools tab. Much more thorough than Drawing View Tracker and you can update everything from the tool!
This can be a big annoyance with many possible causes which even after you fix it you find it often recurs next time you open that draft.
I've worked on drafts where no one else is working on any of the models in the project. I fix it in a session today and it's back the next day.
Plus, in a managed environment you often don't have the capability to fix or regenerate released models that are in your current assembly. So, you live with the grey corners in drafts and the occlusion of annotations and things while working on the draft.
I would like there to be a setting where you can lighten the shade significantly or turn them off altogether in your current session.
my sequence for checing for errors is as follow..
1-"tools" "errors" see what is noted and fix.
2- activate all parts
3- update any mirrors in assembly
4-update all active parts.
Most of the time i'll have a simpe error that i din't notice in a part file 3-4 sub assemblies deep
Someone wrote a macro to handle this problem several years ago. I had it and it worked well at the time, but I am not sure if it will still work with newer versions of SE. I am pretty sure it was developed before the ST era.
I will have a look to see if I can locate it and post it.