Change the parent part and config of a drawing view 1

[CADone]

Hi all,

I have a Sw part A with configs A1, A2 and A3
and a SW part B with configs B1, B2 and B3

Both parts are precisely same without any dimensional changes.

Ihave created drawings with multiple views for A1, A2 and A3. I want to know is there any way I can redirect/change the reference on these drawings that they will be linked to B1, B2 and B3 instead.

I have tried few methods, but they didnot work well for me. All the dimensions were dangling.

Any help on this is highly appriciated.

Thanks
BMR

 

[CorBlimeyLimey]

There are several methods;

SolidWorks Explorer offers Pack and Go, Rename and Replace.

In the File > Open dialogue box, single click to highlight (not open) the drawing file, then select the References option (Lower RH corner). Double click on the component to be changed, and select the component which replaces it. Repeat for all references and select OK. Next, open the drawing file and save it to ensure the references are updated.

There are other "less clean" methods, which force SW into asking for replacements, but the above methods are recommended.

 

[CADone]

CBL,

Thankyou very much for your suggestions.
When I try this I have these following problems:

1. I am expecting views on A1 to be automatically linked to B1. This doesnt seem to happen. On couple of views on the sheet SW uses the last saved config in the part B.

2. Few views which have sucessfully linked to respective configs with part B, have many dangling dimensions.


I can fix the point#1 the hard way. Point #2 is still painful.

Any suggestions are appriciated.

Thanks
BMR

 

[EEnd]

Try this:
[ol][li]Open Drawing A.[/li]
[li]Open Part A. [/li]
[li]SaveAs Part A to Part B. SW will ask if you want to replace references in open documents. Say Yes. NOTE: This will overwrite Part B, but you said that they were precisely the same. Leave the new Part B open. [/li]
[li]SaveAs Drawing A as Drawing B. Leave the new Drawing B open.[/li]
In Part B, rename configs A1, A2 & A3 to B1, B2 & B3. Drawing B should update to the new config names, but if it doesn’t you can redirect them using the view properties.
[li]Save Part B. [/li]
[li]Save Drawing B. [/li][/ol]

Eric

 

[MDGroup]

BMRAO,
Assuming your statement 'Both parts are precisely same without any dimensional changes.' is true, you could do the following.

Open Part A and Drawing A (important to have both open at the same time)

In 'Part A', select save as 'Part B'. This will update all of the drawing views to reference the newly saved 'Part B'.

Go to 'Drawing A' and Save as 'Drawing B'

You should end up with 'Drawing A' still only referencing 'Part A' because you didn;t save over the originals. And now you have a new 'Drawing B' referencing a new 'Part B'

Concerns:
1) As noted above, this assumes Part A and Part B are to be completely identical.

2) If there are drawings/assys that referenced the original 'Part B', now that you have saved over the original with a new 'Part B' you may lose associativity, and any drawings of the original 'Part B' likely wont update correctly.

Hope this helps.

 

[dgowans]

Another thing to be aware of when changing the drawing references: even if the geometry of parts A and B is absolutely identical, your drawing will get hosed if the view orientations between parts isn't the same (e.g. the front view of part A is the same as the right view of part B).

If the two parts are identical but were created uniquely (part B wasn't created by copying part A) you will in all likelihood end up with a bunch of dangling dimensions no matter what you do.

 

[CADone]

I see that few of you are atempting to make a save as of parts and drawings, which is not in my present scenario.

Let me make some points clear with what I have currently.

1. I already have parts A and B ( I dont want to make a Save as)
2. I have drawings for all configs of part A. I want to change the reference of these drawings to be linked to configs of B (I dont want to make a save as B)

Thanks
BMR

 

[ctopher]

CorBlimeyLimey's suggestion should work for you. If not, what issues are you running into?

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[CADone]

I tried what CBL suggested, My issues are.

1. I am expecting views on A1 to be automatically linked to B1. This doesnt seem to happen. On couple of views on the sheet SW uses the last saved config in the part B.

2. Few views which have sucessfully linked to respective configs with part B, have many dangling dimensions.


I can fix the point#1 the hard way. Point #2 is still painful.

Any suggestions are appriciated.

Thanks
BMR

 

[ctopher]

You will have dangling dims because it is now a different part in the view.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[CorBlimeyLimey]

We understand that you already have Part A and Part B, but if they are identical as you stated, it would not matter if you do a Save as over them. That method will work.

Was Part B created independently from Part A? If so that is why you are seeing the dangling dimensions. If it was created separately the face IDs will probably not be the same. Creating Part B from Part A will eliminate that problem.

 

[dgowans]

1. I am expecting views on A1 to be automatically linked to B1. This doesnt seem to happen. On couple of views on the sheet SW uses the last saved config in the part B.

The configurations shown in the respective views will only link if the configuration names are identical. If you can't change the configuration names, you're stuck doing it the hard way.

2. Few views which have sucessfully linked to respective configs with part B, have many dangling dimensions.

Were the two parts created as stand alone parts that have now evolved into the same geometry? If so, you will have many dangling dimensions. If part B was created by copying part A, you might be able to change the references in the drawing and have the dimensions not end up dangling. It all depends on what has happened to the model since it was copied originally. As CBL stated, if subsequent modeling operations have caused the face/edge IDs to change you will have several dangling dimensions.

 

[Standing]

CorBlimeyLimey,
Thank you. Your method works for us, in SolidWorks 2008 sp3.0
A star for you.


Bradley
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