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Alter configuration naming convention

Question asked by Donald Grunloh on Nov 7, 2014
Latest reply on Dec 8, 2014 by Donald Grunloh

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Is there a way to alter the automatic naming convention of part configurations?

We design primarily sheet metal parts. By default SolidWorks names the top-level configuration "Default" and the derived flat pattern configuration "DefaultSM-FLAT-PATTERN". Our drawing sheet names are based off the configuration name, so our designers consistently have to rename each configuration "default to Fabricated" and "DefaultSM-FLAT-PATTERN to Flat-Pattern" Renaming configurations does not always happen so I would like to eliminate the extra naming step for the designers.

SolidWorks 2014 SP 4.0

Daniel Andersson Nov 21, 2014 2:40 PM

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Hi Donald!

I have updated the macro. As I always say... test it!

The naming of the sheets is now according to used configuration. I also added the message if a drawing view have an unexpected configuration reference.

It is easy to turn of, just remove or comment the line with CheckReferencedConfigurations.

Please let me know if things work out as expected or if any further tweaks is needed.

// Daniel

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Glenn Schroeder Nov 7, 2014 1:34 PM
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I don't know for sure if this will work, but it's worth a shot. Start a new Part, and create a simple sheet metal body. Re-name the configurations as wanted. Delete the body, then save as...Part Template. Start a new part with this template. Again, I'm not sure it will work since I don't do sheet metal, but I've re-named my primary configuration as just "Default", and it sticks, so I assume it would work for sheet metal parts also.
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Donald Grunloh @ Glenn Schroeder on Nov 7, 2014 2:37 PM
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Glenn,

Thank you, I am now 50% of the way there. Naming the parent configuration of my part template as "Fabricated" worked perfectly. Creating a dummy sub-configuration "Flat-Pattern" in the part template did showed up in my new parts, but sheet metal automatically creates a flat pattern configuration so I ended up with two sub configurations one called "Flat-Pattern" that was tied to nothing, and another called "FabricatedSM-FLAT-PATTERN" that was tied to the flat pattern. I am still closer than before
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Glenn Schroeder @ Donald Grunloh on Nov 7, 2014 3:25 PM
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At least now you'll only need to re-name one of them instead of two. I'm sorry I couldn't be more help.
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Daniel Andersson Nov 7, 2014 5:47 PM
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The manual renaming could be eased by making a macro. Then the designers just have to click an icon instead of manually renaming the configurations.
Would that be something that you think would be usefull? I might have something early next week.
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Deepak Gupta @ Donald Grunloh on Nov 8, 2014 12:43 AM
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SW renames/create flat configuration with the name"ConfigNameSM-FLAT-PATTERN". I'm not sure if there is option to change that permanently.

You may rename the config name but can't you keep the flat pattern config name as it is. BTW how are you renaming the sheets; I believe manually OR via a macro OR do you have the drawing template setup with sheet renamed to require named.
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Daniel Andersson Nov 8, 2014 6:13 PM
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Hi Donald,

If you like, try out this macro. It will work on parts and drawings. I made this macro since this topic has been raised from time to time in the forum.
The Macro renames the "Default" configuration and the "DefaultSM-Flat-Pattern" etc etc. More details is found in the macro file.

These are the variables that you can play with...

sDefaultOld = "Default" 'Old name...
sDefaultFlatOld = "DefaultSM-Flat-Pattern" 'Old name of Flat-Pattern...
sDefaultNew = "Fabricated" 'New name...
sDefaultFlatNew = "Flat-Pattern" 'New name of Flat-Pattern...

Quite simple, the "old" variables will be renamed to the "new".
The macro will only rename configurations found in part (a) or in part that is referenced in drawing view (b).

(a) Macro executed with a part as active document.
If the macro is executed with a part as active document, the matching configurations will be renamed.

(b) Macro executed with a drawing as active document.
If the macro is executed with a drawing as active document, the macro will process each view and
check if the view has a part with matching configuration. If there is a match, the macro will open
the referenced document silent and rename the configurations and then switch back to the drawing.

Pay attention that the macro DO NOT consider ANY references to other parts, assemblies or drawings.

Note that the macro will rename any "Default" configuration in a part (or refereced part from drawing view), no matter if its a sheet metal part or not.
Further checks and controls can be added to control this in a better way...

This would replace the manual work with pressing a button instead. See this SolidWorks help topic for details how to add a button.

Please let me know if you tested the macro and how it worked out for you. (And make sure to have back-ups of the files that you try the macro at first.)

EDIT: It just hit me that it is quite easy to check if a view is flat pattern. Let me know if you want the macro and then I can update it to only apply changes on referencef parts in flat pattern drawing views and not all views as today.
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- RenameFlatPattern1.zip15.8 KB
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Donald Grunloh @ Daniel Andersson on Nov 10, 2014 7:30 AM
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Thank you everyone for their input, I greatly appreciate the help.
Currently we are manually renaming the drawing sheets to match the configuration of the part. A macro to rename configurations would work just as well.

Daniel,
I will try out the macro here with our designers, and I will report back. Thank you
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Deepak Gupta @ Donald Grunloh on Nov 10, 2014 7:45 AM
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You can also use the macro to rename the sheets also.
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Donald Grunloh @ Deepak Gupta on Nov 10, 2014 9:04 AM
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Deepak,
Are you indicating that the macro Daniel posted can change the sheet names as well, or that a similar macro could be created to perform the action of renaming sheets?
I am not very familiar with visual basic, but looking at the macro Daniel posted the change configuration function only addresses models, not drawings.
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Daniel Andersson @ Donald Grunloh on Nov 10, 2014 9:39 AM
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It is possible to extend the macro to have functions to rename sheets as well.
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Deepak Gupta @ Donald Grunloh on Nov 10, 2014 10:05 AM
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Yes and Daniel confirmed it. So simply open the drawing, run the macro and get everything renamed
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Donald Grunloh @ Daniel Andersson on Nov 10, 2014 1:51 PM
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Having the sheet rename function as well would answer all of my needs. Would it be possible to post an updated macro or secondary macro to include the sheet rename function?

I have very little VB skills so I greatly appreciate everyone's help and comments on this topic.
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Daniel Andersson @ Donald Grunloh on Nov 10, 2014 3:39 PM
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I'm currently a bit short of time and I think I would change to approach of the code to add renaming of the sheets.
I could update the macro but not until the next weekend. Perhaps someone else can edit the macro before that. Otherwise I will make an update next weekend.

Just to catch a few details...
Has the drawing sheet with the flat pattern only a flat pattern view or do the engineers add a iso view of the fabricated product there as well? I'm thinking of a way to find out which sheet that should be name Flat-Pattern. Currently I thinking of having the flat pattern view as a trigger for this.. which means that if the engineer has put a fabricated view and a flat pattern view on the same sheet, the sheet name will be Flat-Pattern.

// Daniel
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Donald Grunloh @ Daniel Andersson on Nov 11, 2014 7:36 AM
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The current macro that you created is a huge advantage already. This is not a rush item, so if you want to work on it do so as time allows.

The majority of the parts will have a fabricated view on sheet 1, and flat-pattern view on sheet 2. Very rarely would our engineers combine a fabricated view and flat pattern view on the same sheet, but if they did there would be an fabricated iso view. Similarly there are cases when our engineers may put fabricated views on sheet 1 and sheet 2, then flat pattern on sheet 3, but this is rare as well.
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Daniel Andersson @ Donald Grunloh on Nov 13, 2014 4:35 PM
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Hi Donald Grunloh
I had more time this week than I thought..!
Made an update of the macro, please test run it and be abusive to it... so you can find out if there are any bugs or strange behavior.

The macro is changed a bit but works in the same way... there is two new variables to set for the sheet names:

sDefaultOld = "Default" 'Old name...
sDefaultFlatOld = "DefaultSM-Flat-Pattern" 'Old name of Flat-Pattern...
sDefaultNew = "Fabricated" 'New name...
sDefaultFlatNew = "Flat-Pattern" 'New name of Flat-Pattern...
sSheetNameFlat = "Flat-Pattern" 'Name to be set to each sheet with a flat pattern view + index number (start at 1)
sSheetNameNonFlat = "Fabricated" 'Name to be set to each sheet without a flat pattern + index number (start at 1)

One thing to be aware of is that the renaming of configurations will only be done if the current configurations has names as stated in the ..Old variables. I had some thoughts about it since it is possible to just push what ever name you want. But I think it is good to not do that, since there might be mixes / variations of other names. I see it as a higher risk for conflicts of the configuration names. But I just wanted to mention that so you are aware of the requirement that the configurations must match the strings as stated in the ...Old variables.

Renaming of the sheets is done, and if there is one view with flat pattern the view will be renamed to Flat-Pattern 1 (or what ever name is set in the sShetNameFlat variable).
I added index / numbering to the sheets to avoid conflicts of the name. The index currently starts and shows at 1 (one).
e.g. "Fabricated 1" and the second "Fabricated 2" and then flat pattern "Flat-Pattern 1".

But it could be changed with some tweaks, to be like this "Fabricated" and the second "Fabricated 2" and then flat pattern "Flat-Pattern".

And finaly I want to push for this note once again... since assemblies or other drawings might not find the configurations due the renaming.
Pay attention that the macro DO NOT consider ANY references to other parts, assemblies or drawings.
This is a part of the consequents that I have not been looking into. So I recommend that you test out and see how an assemblies behaves after the the part has the configurations renamed. (To test it, open part or drawing, run macro, save and close, open assembly... what happens?)

Please let me know how the testing worked out.
// Daniel
Attachments
- RenameConfigAndSheet2.zip19.8 KB
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Donald Grunloh @ Daniel Andersson on Nov 14, 2014 7:43 AM
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Thank you very much Daniel. I will start testing out the script immediately and report back if I notice any bugs or odd behavior.

Don
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Donald Grunloh @ Daniel Andersson on Nov 14, 2014 9:46 AM
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Daniel,
Found a couple of bugs so far. Ill do my best to explain them, but if there is a better way to relay the information let me know.

Action: Created a new sheet metal part and saved the document. Then went to file -> make drawing from part. I then created a drawing with two sheets. Sheet 1 contained the part in it's bent state. Sheet 2 contained a view of the part in its flat-pattern state. Note at this point I have not run the scripted so the part's configuration names are still the default names. At this point I ran the latest script to rename both the part's configuration and the sheet names. Following things took place

1. Error message window popped up stating "Configuration "fabricated" already exists in document.........." and "Configuration Flat-Pattern" already exists in document....." I imagine that the script is renaming the part configuration, then looping back and trying to rename the configuration again causing this message to pop up.

2. Both sheets are labeled as "Flat-Pattern". Even though sheet 1 only has a fabricated view, and sheet 2 only has a flat-pattern view both sheets are labeled as "Flat-Pattern"

I performed the same action again but this time after creating the drawing I ran the script with the part first to rename the configurations. I then ran the script a second time with the drawing to rename the sheets. I ran into the same errors and before.
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Daniel Andersson @ Donald Grunloh on Nov 14, 2014 4:49 PM
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Thanks for the detailed feedback. I will look into this during next week.

1) It seems like I complicated one thing error messages. They should only be triggered from the referenced part and not drawing as to day.

2) I have tried to replicate this bug with no success. But I see that there is some odd behaviour with an array...
I was able to replicate the error at last, even more strange things was going on when I switched places of sheets. For some reason the API return views that is on other sheets as well. I will filter this by using IView::GetVisible. This means that the view will not influence the macro if its hidden (by user or system).

I also see that it is important that the drawing has been saved one time (there must have a vaild path to a file) before executing the macro. Otherwise it will not switch back to the drawing after updating the configurations in the part. I will add a message that allows the uset to select to save if needed or exit the macro in a more controlled way.
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Daniel Andersson @ Donald Grunloh on Nov 14, 2014 5:03 PM
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I have updated the macro, please make a new test run.

Currently it is not required to save the drawing. Since the macro uses the title of the document and not the file path. Usually this is not a good solution since depending on settings, the title can be same as for part and assembly and even for drawing if you push it a bit.. But I think we are Ok since we use the title for a drawing document, there is not many people naming thier part/assemblies and drawings as "partno - Fabricated 1" etc etc.

I also removed the error messages as explained previously... they was not needed.

I also want to clearify the renaming of the sheets.
The naming of the sheets is controlled by using the flat pattern view in the view properties.
So it is currently possible to make a sheet with views and use the regular orientations and set the configuration to "DefaultSM-Flat-Pattern" or "Flat-Pattern".
This would still look like a flat pattern drawing view, but the views is not real flat pattern views in SolidWorks terms and the macro would assign the sheet a "Fabricated..." name.
Depending on your process how you use the views, I can make the macro to rename the sheet to "Flat-Pattern..." depending on configurations and/or the SolidWorks view type.
Just let me know.

SolidWorks creates another ....SM-FLAT-PATTERN configuration
Using this options also leads me to the latest finding... SolidWorks loves to create the ...SM-FLAT-PATTERN configuration.
If configurations "Fabricated" and "Flat-Pattern" exist, SolidWorks will create "FabricatedSM-FLAT-PATTERN" if the user inserts a new flat pattern view if the user have selected "Fabricated" configuration before checking the check box for view (A) Flat pattern.

Amazing isn't...? So the user must have an eye on which configuration that is selected before they choose view. Below is a screen from how it might look...
Depending on how you create views today, you already might have this issue already. We could have the macro to clean this up as well...

Bash the macro a bit and see if something fails and let me know you thoughts about me comments above.
A update of the macro due to the information above might be needed, just let me know.

Best regards
Daniel
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- RenameConfigAndSheet2.zip21.3 KB
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Donald Grunloh @ Daniel Andersson on Nov 17, 2014 8:59 AM
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Thank you Daniel,
I just tested out the script quickly things look great!! I will be putting the script through its paces this week here and report back with any odd behavior.

The engineers like the script as well. Only change request they have so far is eliminating the index number on first sheets (so first sheet would read "Fabricated" not "Fabricated 1". I found the function that assigns the sheet name and tried to add the following if statement. This eliminates the index number from first sheet, but labels the second sheet as "Temp Sheet 2"

Restart_:

    sNameTemp = sName & " " & k

    For i = 0 To UBound(vSheetNames)
        If sNameTemp = vSheetNames(i) Then
            k = k + 1
            GoTo Restart_:
        End If
    Next

    If k = 1 Then
        sName = sName
    Else
        sName = sName & " " & k
    End If

    SetSheetName = sName
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Daniel Andersson @ Donald Grunloh on Nov 17, 2014 2:25 PM
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You are close. But since the loop goes back to restart, you have to add a IF statement at the restart.
Since sNameTemp is used to check the sheet names that is currently in the drawing. sNameTemp must represent the logical order of naming the sheets.

Update the macro with this...

Restart_:



    If k > 1 Then

        sNameTemp = sName & " " & k

    Else

        sNameTemp = sName

    End If



    For i = 0 To UBound(vSheetNames)

        If sNameTemp = vSheetNames(i) Then

            k = k + 1

            GoTo Restart_:

        End If

    Next



    If k > 1 Then sName = sName & " " & k



    SetSheetName = sName
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Donald Grunloh @ Daniel Andersson on Nov 19, 2014 9:22 AM
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Thank you!

I have been playing around with the script for a bit here and so far things are working very well. Talking with the engineers when creating a drawing they sometimes select the configuration name rather than the view when creating a flat pattern sheet. By selecting the configuration rather than the view the sheet is labeled as fabricated, just as you indicated in an earlier post. If the script was altered to look at the configuration name rather than the view name would the error still exist but now in revers? Meaning that sheets made with flat pattern views will be labeled as fabricated, but sheets made with flat pattern configurations would be labeled as flat-pattern?
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Daniel Andersson @ Donald Grunloh on Nov 19, 2014 2:01 PM
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1) There would not be an reversed error if we go for using the configuration name instead of the flat pattern view.
The only thing with that, is if the configuration name is something else than expected, then the sheet name would be Fabricated.

Having a second thought about it, it might be better to use the configuration name to set the name of the sheet.

2) A new idea popped up... would it be good information to give the user if an unexpected configuration name was found in one of the views?
E.g.
Unexpected configuration name
An unexpected configuration name was found in view XX on sheet YY.

Just let me know and I will update the macro.
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Donald Grunloh @ Daniel Andersson on Nov 20, 2014 9:03 AM
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If it would not break things naming the sheet based on the configuration would be optimal since it allows flexibility to add views to a drawing in multiple methods. I like the idea of the error message as a backup to potential issues for our situation. Would it be possible to add the error message function with the option to comment the function out? If we run into an issue where the error message becomes more annoying then helpful it could always be turned off.
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Daniel Andersson @ Donald Grunloh on Nov 21, 2014 2:40 PM
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Hi Donald!

I have updated the macro. As I always say... test it!
The naming of the sheets is now according to used configuration. I also added the message if a drawing view have an unexpected configuration reference.
It is easy to turn of, just remove or comment the line with CheckReferencedConfigurations.

Please let me know if things work out as expected or if any further tweaks is needed.

// Daniel
Attachments
- RenameConfigAndSheet23.zip22.3 KB
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