copying assembly models

[Tenkan]

I created an assembly model from three components. I made all three components virtual. I then added two more components as virtual parts to complete the assembly and then created the drawing. When I was finished I closed everything and then copied the assembly model in windows and renamed it to another part number that is almost identical.
My problem is, I now cannot edit the components in the new/copy assembly model. The error I get says "this part has features defined in the context of another assembly<original assembly.sldasm> You can edit the part, but cannot create any external references to the components of the current assembly".

Which is exactly what I need to do....

What are my best options here to replace the link with the original assembly model to the new one?

lightweight, cheap, strong... pick 2

 

[ctopher]

The problem is you used Win Explorer to do it. Use SolidWorks Explorer to copy/rename/etc your files.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[Tenkan]

Thanks Chris I am giving that a try it seems to help but pasting in SW Explorer (SWE) is not straight forward.

I should note the company I work for does not have PDM works... This is my first time working without PDM in years so...

So i copied the file from SWE but had to paste it into windows and when opened the new 'test' copy had the same issue. So using SWE is not helping unless I find find a way to paste without using pack and go...

I was hoping that when I copy/duplicate an assembly model the internal virtual parts external references move with the copy. Im surprised they stay linked to the original file!!!! What I had to do was manually remove all the references from the features and sketches and re-do them. (I did that because I hate leaving the ->x symbol in my work).





lightweight, cheap, strong... pick 2

 

[laik]

Hi,
You could try this:
In SolidWorks open your assembly with virtual components.
1. Select File - Pack and Go - Select Include drawing - Type a new file name as indicated in the attached picture - Save.
You can also use Pack and Go in Solidworks Explorer.

 

[Nella95]

I use SW Explorer - but I think you can right click on the assembly/drawing in Windows Explorer, and select 'Pack & Go.' Try that too.

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[CorBlimeyLimey]

... but pasting in SW Explorer (SWE) is not straight forward

So i copied the file from SWE but had to paste it into windows

What are you pasting, and why?

 

[Tenkan]

To follow up with this I found the solution, is within Solidworks. Don’t ‘save-as’ from Windows, open the assembly in Solidworks and save-as from there. Rename the file and hit save and the save happens you will get a dialog box pop up that will explain the links issue and give instructions to link the virtual components to the new assembly proper…

lightweight, cheap, strong... pick 2

 

[mjcole]

Solidworks Handles File References horribly when performing simple Save As Copy Or Rename from within the product without Using the Pack & Go option on the File Menu.
Even when using pack and go it has been super buggy at times but allows you to replace your references and save to new names during the Packing process. Solidworks doesn't update the Relations between parts properly because they only really work on the original files.

SolidWorks should be giving warning messages warning about this error you are seeing possibly happening when doing the Save As.
Unless you fully understand the relations between parts and even if you do it's a good idea to still use at least SWExplorer and better yet Pack & Go if SolidWorks is up and running. See if you can get your hands on a File Management Training manual if anyone you know has taken that because it will have many answers to your questions.

If you are really desperate you can take a Training Class at your VAR but it probably costs way more money than it's worth imbo (boastful opinion).

Although If You are on subscription definitely talk with one of their Top AE's (Application Engineers) about your specific issue and get a Best Practices document made to avoid issues like this in the Future.

Another thing that may work at this point is to Select Your Win-Explorer copied Assembly file and before opening hit the
[References] button in File Open dialog.
This will give you a list showing all the parts & assemblies in your badly copied Assembly and it's original referenced files. From this dialog you can double click in the Prev Filename column on any files which you want to replace with your copied ones new names and The old reference will be switched to the new file names when you open the copied file by this method.

I originally had problems like this when first learning SolidWorks but now that I've been using it for 10 years I know to avoid doing any dodgy windows explorer file renaming.

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