Replace part/assy in dwg 1

[ctopher]

I don't have 2006 yet. Do you guys know if you can replace an assembly with another assembly in a dwg with SW 06?
I have a complicated dwg with a big assy. There is a new assy that is 90% like the other. I would like to replace the old with the new and rename the dwg for the new.
thanks

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[J-C]

You can do that any any version of Solidworks, unless I'm missing something.

Jason

 

[SBaugh]

You can do this with SW explorer any version.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[miller7778]

How do you do this?

 

[J-C]

In Solidworks:

Select File/Open
In the open dialogue, select and highlight the drawing, then select the "references" button.
Double click the assy path shown and browse for the new assy.
Ok that and the "Ok" to open the drawing.


In Solidworks Explorer:

Open drawing file.
In the tree, right click the assembly and select replace.
Browse for new assy
Apply

Jason

 

[SBaugh]

IN SW explorer you

1) open the Drawing
2) select Edit\Replace
3) Highlight Assembly
4) Select "Browse" and browse for new assembly
5) You can do a "find where used" if the assembly is used elsewhere, recommended if you do this to parts.
6) Select "apply"

If you have anything in the Find where used box there they will turn blue, informing you they have been updated.

Regards,


Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[smcadman]

I do it in Solidworks, not SW Explorer.
see thread 559-122252
"Drawing reference: Was assembly, is Part"
This should be in the FAQ because it has been asked a few times, but in different ways.

Flores

 

[SBaugh]

Then make an FAQ out of it, but include all the ways not just from SW side, because I have been using Explorer and if you have in-contexted part files and you change a name... doing it from SW alone will not update the files that the part is associated like SW explorer does.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[J-C]

I have to agree with Scott.
Swx Explorer is the best way to visually see what's going on and provides more options for maintaining references, where-used, etc.

Now if Solidworks would just replace the "References" button in the Open/Save dialogue with a revamped Explorer interface. Time for an enhancement request.

Jason

 

[ctopher]

I have been trying to do this with SW Exp, but won't work for me. It works well with replacing/renaming in an assy, but not in a dwg.

Gildashard, the open/file references worked! perfect!
thank you

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[Heckler]

I'm with Scott, That's why SWx Explorer was developed. This is what the SWx help has to say.

The SolidWorks Explorer is a file management tool designed to help you perform such tasks as renaming, replacing, and copying SolidWorks files. You can show a document’s references, search for documents using a variety of criteria, and list all the places where a document is used. Renamed files are still available to those documents that reference them.

NOTE: The SolidWorks Explorer is not a PDM (Product Data Management) tool; however, it does perform many useful tasks and simplifies many file management processes.



Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[ctopher]

Scott and Heckler,
I agree with you guys 100%.
I use SW Explorer all the time for various issues.
But the only thing it won't do for me is replace a part/assy in a dwg. Time for another Enh Req.
thank you for your help

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[smcadman]

Swx Explorer is the best way to visually see what's going on and provides more options for maintaining references, where-used, etc.

I know there is more than 1 way to skin a cat, but how can you visually see what is being replaced? I only get the first page on a drawing. I cannot see page 2 or page 50 for that matter.

I use SW Explorer all the time for renaming files, changing properties, etc. because of the "find where used" feature. I just haven't used it for repacing Asm. A with Asm. B on a drawing.

As for replacing a part or sub-assembly in an assembly within SW, I right-click what I want to replace, and pick "replace components".
Cheers I

Flores

 

[J-C]

Well the drawing in your case is referencing one assembly (assy a). And you can replace it with assy b, but it does so for all sheets. Sounds like you want to just replace certain views on the drawing with another assy while leaving the rest of the views referencing the first assy.

I've only had to do this once. I think what I did was save a copy of the drawing. Then replaced the copy's assy with the second assy. The cut and pasted the views in the copied drawing file back into the original. Now the drawing is pointing to two assembly files.

Jason

 

[SBaugh]

ctopher,

It's just the user bud (no offence), no need for an ER. I just made an avi file for you to look at and show you how it's done.

I sent it to your yahoo address from your home website.

Check it out.

Best Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[ShaggyPE]

smcadman
"I do it in Solidworks, not SW Explorer.
see thread 559-122252
'Drawing reference: Was assembly, is Part'"

That thread that you mentioned was a bit of a special case that I believe is still not possible; Changing the reference of a drawing from a assembly to a part.

Anybody with 06 give this a try?

 

[ctopher]

Thanks Scott.
I tried that per your video, but for some reason doesn't work for me...never has. It works well for replacing a component in a assembly, but not a dwg.
I may have to reload SW Explorer, maybe it will fix it.
thanks again.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[smcadman]

That thread that you mentioned was a bit of a special case that I believe is still not possible; Changing the reference of a drawing from a assembly to a part.

You started that thread, and neither SW, or SW Explorer worked for you, but I have done this several times. After reading the steps you took, I see what you were doing wrong: You opened the DRAWING FIRST, and then tried to do a reference change.
The correct way is BEFORE OPENING THE DRAWING, in the Open dialog box, pick the drawing (not open), and the lower right-hand side hit the "References" button. From there is where you can double-click a specific page and change the reference.

Yours was a simple assembly with sheet metal + pem nuts. Not only have I replaced the assembly with just the sheetmtal, but I have changed square tubing that had Riv-nuts to just the part with no Riv-nuts.

Flores

 

[ShaggyPE]

smcadman,
What version of SW are you using. As per the former thread (thread559-122252), I did exactly as you state, clicking references BEFORE OPENING THE DRAWING and I select the part that I want to replace the assembly with. It fills in the path, the way it should, but when I select OK, I get an error message. I am using SW2004 with the latest service pack.

Does this work with a newer version? I haven't tried with 2005 at home.

I have done the references replace game many times, but it only works part to part or assembly to assembly, not part to assembly. This is in the context of opening a drawing of course.

 

[smcadman]

Shaggy,
I am using SW 2005 SP 4.0. Don't know why it isn't working for you, because I have done this on several occasions. Typically it is when a client wants to save money and wants a thru-hole and will use nuts and bolts instead of paying for the pem nuts or riv-nuts as well as the labor to install them.

Flores