CAD Forum

This may be an easy one for someone who knows.
How to change all drawing views in an existing drw file to a different configuration of a multi-body weldment part, and assign all balloons to a new weldment list, at the same time.?
Rather than individually on a one-by-one basis.!

For the configuration, a few ways i can think of at the moment... (others should have some better idea)

Option 1: Using Properties
You can shift select all your drawing view, right click and select properties, after that you can change the configuration for all the view selected at once.
However, this only work for 1 sheet at a time, if you have multiple sheet, you will need to perform on all Option 2: Using Replace Model with a intermediate dummy part
Replace Model allows you to change the model and configuration at the same time for all the drawing view.
https://help.solidworks.com/2021/englis ... _Views.htm
However, it will not work if the file name/reference is the same. The workaround will be using an intermediate dummy part.
To do that:
1. Select Replace Model
2. Select All view
3. Browse and select the intermediate dummy part (eg: Dummy.prt)
4. Select Replace Model again
5. Select All view
6. Browse and select your original file, select the configuration in the open window

This might break something unintentionally Option 3: Macro
You can create a macro that iterate through all drawing view and change the configuration.

The bom is a bit tricky though because if your face or edge ID change it might not be recognize anymore.

Zhen-Wei Tee wrote: ↑Wed Sep 14, 2022 6:46 am Option 1: Using Properties
You can shift select all your drawing view, right click and select properties, after that you can change the configuration for all the view selected at once.
However, this only work for 1 sheet at a time, if you have multiple sheet, you will need to perform on all
image.png

Yes. This seems to be about the best way to go. At least, without breaking anything.

Meh. I had hoped there was an easier way than trolling thru multiple pages.
Even so, this is still easier than creating a whole new drawing file tho, so there is that.

Cheers Zhen.

Hey Damo, I can most likely help you.

You can change the file that is used in a drawing using File>Open>References
You can also use this macro, I believe provided by @gupta9665, to select the desired table to be used on which sheets/views for balloons.

I don't think you can pick the configuration when using File>Open>References

It works great for swapping one part or assembly with another and not having to do the drawing from scratch, especially on parts where you do a save as and make it a new version of a similar part.

TTevolve wrote: ↑Fri Nov 18, 2022 8:59 am I don't think you can pick the configuration when using File>Open>References

It works great for swapping one part or assembly with another and not having to do the drawing from scratch, especially on parts where you do a save as and make it a new version of a similar part.

Indeed, but if his multibody part is made from the previous multibody part that was used for that drawing, then most likely when he does the switch in reference everything will follow through with the right configuration selected, which is what it sounds to me like he is trying to do.

AlexLachance wrote: ↑Fri Nov 18, 2022 9:27 am Indeed, but if his multibody part is made from the previous multibody part that was used for that drawing, then most likely when he does the switch in reference everything will follow through with the right configuration selected, which is what it sounds to me like he is trying to do.

I got a little excited by this...

I wondered if just maybe it was crazy enough to work.
(Small caveat. All these attemps at this were done on a "Copy of the project folder" I do not want to break my working files.)
And so, if I understand your meaning correctly, save my multi-body part with the same name but in the new configuration. Then close the part.
Now use the open file dialog to select the drawing file, (and yes, as was stated by TTevolve, you cannot select the configuration of the part to open),
When selecting the referenced part to open, I selected the same part, in the hope that the SW would indeed assume to load the most recently saved configuration into the drawing file.. But Alas, it is not to be.

I also tried to save the part with a new filename and then open the drawing file by referencing the newly named component..
Indeed it did open the newly named part. But retained the configuration that the views (and cut-list) were previously associated with.
In fact, I tried opening the newly named part with all other configurations deleted. Something in the way SW retains references meant it stubbornly refused to accept the file I stipulated and opened the original file with the unwanted config anyway.
The only success I did have, was to rename the original folder, delete all other configs within my copied file (of the original name) and then the refences process of the drawing file open did yield success. The original config could not be found and so the SW opened the file with the only config it could find.
This was interesting in that it did indeed acheive the effect of all views displaying the correct config.
But many views were of course broken with dangling dimensions and missing bodies, or displaying unwanted bodies.
This is expected behaviour and this happens when manually changing view configs anyway tho.
And interstingly, the cut-list was broken completely. All balloons reverted to "1" and the cut-list could not be attached to the new config.
A new cut-list quickly fixed this tho.

In short. This is something than is somewhat workable.
The amount of work to repair the individual views for a different config will be dependant upon how much diffence there is between the configurations.
This could indeed be more work than simply reconfiguring views.. But it could also be much less work.

Today, I have learnt something. Thank you guys.

Damo wrote: ↑Mon Nov 21, 2022 12:08 am I got a little excited by this...

I wondered if just maybe it was crazy enough to work.
(Small caveat. All these attemps at this were done on a "Copy of the project folder" I do not want to break my working files.)
And so, if I understand your meaning correctly, save my multi-body part with the same name but in the new configuration. Then close the part.
Now use the open file dialog to select the drawing file, (and yes, as was stated by TTevolve, you cannot select the configuration of the part to open),
When selecting the referenced part to open, I selected the same part, in the hope that the SW would indeed assume to load the most recently saved configuration into the drawing file.. But Alas, it is not to be.

My apologies, the drawing does not pick up on the most recently saved configurations, it picks up on the existing configurations that were used to create the drawings. If the configurations from Part A have the same name as Part B, then you can use the drawing of Part A to partially generate the drawing of Part B.


The only way SolidWorks will change a drawing view's configuration without user interference is by doing what you stated; deleting all the configurations so that the drawing has no choice but to load the desired configuration. Though, I doubt that is what you intend/need.


Edit: Maybe you could do a little dance around it. Maybe you'll get the jist of what I'm saying, maybe you won't. It still requires a lot of work, but perhaps it could be simplified.

Have a part file with all desired configurations. (Part A)
Have the same part file with one configuration while making sure it has the same config name as the previous part. (Part B)
Switch the drawing reference from Part A to Part B and save the drawing.
Switch the drawing reference from Part B to part A.


Maybe that would leave you with less stuff to fix, maybe it won't. Just thinking out loud.

AlexLachance wrote: ↑Mon Nov 21, 2022 8:08 am My apologies, the drawing does not pick up on the most recently saved configurations, it picks up on the existing configurations that were used to create the drawings. If the configurations from Part A have the same name as Part B, then you can use the drawing of Part A to partially generate the drawing of Part B.


The only way SolidWorks will change a drawing view's configuration without user interference is by doing what you stated; deleting all the configurations so that the drawing has no choice but to load the desired configuration. Though, I doubt that is what you intend/need.


Edit: Maybe you could do a little dance around it. Maybe you'll get the jist of what I'm saying, maybe you won't. It still requires a lot of work, but perhaps it could be simplified.

Have a part file with all desired configurations. (Part A)
Have the same part file with one configuration while making sure it has the same config name as the previous part. (Part B)
Switch the drawing reference from Part A to Part B and save the drawing.
Switch the drawing reference from Part B to part A.


Maybe that would leave you with less stuff to fix, maybe it won't. Just thinking out loud.

There is definitely something to this.
And very likely a good way to save me some time in the future.
One thing I have learned with SW is that Configurations are not all they are touted to be.
It may just be safer in the long run to create new files (and filenames) from my modified original parts and then simply delete the original configs to attach a copied and renamed drawing file to it.
Then I have both as separate project files. each can be modified individually and independantly without breaking the other, if need be.
I reckon this will actually be less clunky than trying to maintain separate configs anyway.
It is easy enough to "Replace Component" within an assembly too.
And have lighterweight files.

Knowing I can remove all existing configs from the modified file and attach a drawing to it will indeed create the desired effect of having all views display the config I want/need.
This is a workable solution for the time being..

Damo wrote: ↑Tue Nov 22, 2022 6:25 pm There is definitely something to this.
And very likely a good way to save me some time in the future.
One thing I have learned with SW is that Configurations are not all they are touted to be.
It may just be safer in the long run to create new files (and filenames) from my modified original parts and then simply delete the original configs to attach a copied and renamed drawing file to it.
Then I have both as separate project files. each can be modified individually and independantly without breaking the other, if need be.
I reckon this will actually be less clunky than trying to maintain separate configs anyway.
It is easy enough to "Replace Component" within an assembly too.
And have lighterweight files.

Knowing I can remove all existing configs from the modified file and attach a drawing to it will indeed create the desired effect of having all views display the config I want/need.
This is a workable solution for the time being..

Good stuff buddy! If you expand upon the principle, would you mind sharing? It is somewhat a process I use when creating a family of parts using a design table to drive the configurations.

Cheers mate!

AlexLachance wrote: ↑Wed Nov 23, 2022 10:49 am Good stuff buddy! If you expand upon the principle, would you mind sharing? It is somewhat a process I use when creating a family of parts using a design table to drive the configurations.

Cheers mate!

Oooo.. A design table..?! That is fancy stuff I've never really put effort into working out.
But doesn't that involve multiple configurations of a single part (or assy).? (I fear I'm showing more of my ignorance here..)
In which case yes, the issue of drawing files not being able to update to differing cofigurations would indeed be troublesome..

Do you currently create completely separate drawing files for each configuration.?

Damo wrote: ↑Wed Nov 23, 2022 6:45 pm Oooo.. A design table..?! That is fancy stuff I've never really put effort into working out.
But doesn't that involve multiple configurations of a single part (or assy).? (I fear I'm showing more of my ignorance here..)
In which case yes, the issue of drawing files not being able to update to differing cofigurations would indeed be troublesome..

Do you currently create completely separate drawing files for each configuration.?

Indeed. I have some parts that contain around 150 configurations and 150 drawings to go along with those configurations. Here's a simple example of a family of parts incremented by every inch.

RAID-842 is the part
006 is the configuration name/length of the part
The drawing cartridge calls out the file name of the drawing.