SW03 SP5 bug? Really frustrated

[dogarila]

My usual method of duplicating drawings is:

Suppose I have part A1 with its drawing D1 and part A2 identical to part A1. To create the drawing D2 for part A2 I open D1, save it as D2, close it, goto File, Open, click on D2, click on References, change A1 to A2, click ok, click Open. D2 opens pointing to A2.

I use SW03. It worked fine in the past. Since I installed SP5 it doesn't work anymore. Anybody knows an alternate method?

SBaugh says SW will not make another SP for SW04. So those of us who paid big money for SW03 and subcriptions and do not plan to move to SW04 soon, have to use this bugged SW03?

I would gladly return to SP4 but for that I have to reinstall SW03, than install the SPs and customization and I really have no time to do that

 

[SBaugh]

SBaugh says SW will not make another SP for SW04.

I hope you meant SW03? So your saying that those people that are still using SW01+ and they have a bug in that last SP. You think SW should repair that issue? It's probably fixed in SW03 SP0. This also works for SW04. Your problem is probably fixed in SW04 SP0.

Have you tried using SW explorer?

Another alternative:

If you have Drawing D1 open and Part A1 open at the same time. You could save Part A1 to A2. You will get a message telling you that D1 is referencing A1, are you sure? You say Yes. Once the file is saved click to the drawing and let it update. Then do a Save as on the drawing and it to a new name of D2. Now you have a new drawing D2 referencing part A2 and your original D1 and A1 is fine.

If this doesn't work for you, or SW explorer doesn't work for you, and your unwilling to reinstall to SP4. There isn't much anyone can do for you.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[bwagner]

I can confirm that the bug you are seeing is only in SW2003 SP5. It is correct in SW2003 SP4, and SW2004 SP0 and SP1.

I came across the bug the first day after I installed SP5.0. I submitted the report to my VAR, and was told that they believe that SP5.0 will be the last SP for SW2003.

Also, I was told by my VAR the problem is not necessarily considered a bug becasue that is not the "preferred" way to change file references. You are supposed to use SW Explorer for those actions.

I have gone back to 2003 SP4.0 and 2004 SP1.0, without issue.

Best Regards,
Brent M. Wagner

 

[Regg]

bwagner

Sounds like your var is giving you a line of ________ (of course everyone has their opinion as to which is the "right" way to do thing in SW). My VAR had showed me this method as a quick and easy way to do just what netshop21 is trying to do and how to relink a model to a drawing when you change the model name without having the drawing open.

Regg

 

[mncad]

bwagner & netshop,

What OS are you using? I have SW03 SP5.0 on Windows 2000 Professional and I do exactly what you are talking about all the time. In fact I just did it this morning without a problem.

 

[Mandrake22]

Here is a slightly different technique that may work.
1. You have A1 and D1 and want to CREATE A2 and D2.
2. Save D1 as D2. While doing so, click the References button.
3. In the "Edit Referenced File Locations" screen that should now be open, click the box at the far LH side of the file path/name.
4. Change the file path and/or name to A2. You have to do a slow double click to edit this.
5. Click OK.
6. Now select the current path and enter the file name for A2.
7. At this point, you have two identical parts and drawings.
8. Edit A2 to your liking. (make sure you are working in A2 and not A1!)
9. Look at D2 and cleanup as needed.

 

[dogarila]

mncad, I am using Windows 2000 Professional. When did you install SP5?

Mandrake22, your method is OK if you want to CREATE A2. In my case A2 is already created, inserted in an assy and mated. To use your method I have to create first A2a, then open the assembly, replace A2 with A2a, then with D2 open save A2a as A2. All these extra steps mean lower productivity. Who's gonna pay for it?

 

[mncad]

netshop21,

I have now found the same bug. The files I was working with were created in SP5.0. Today I tried a file that was created in an earlier service pack and changing the references in the drawing file does not work now. Have you found anyway around it? I haven't found a way in SW Explorer to do it.

mncad

 

[BBJT]

Sorry if I am eching anyone above but I a to lazy today to read all the replys.

Here is how we do it.

1.) You have a part A1,A2 and drawing D1 that references A1.
2.) When you go to open D1 select References in the open dialog box. Double Click on the new pathname and the browse will pop up. Double click A2, OK, open the drawing.
3.) Be sure and do a file saveas to create your D2 file.

This is fairly quick and easy to remember.

BBJT CSWP

 

[SnowCrash]

When I do this I open the drawing D1 and the part file P1 at the same time.
Make a change in the part and save as P2.
Switch to D1 and regen to check that the ref part is now P2.
Save as D2.
P1 and D1 are still on disk unchanged.
Another way to do repetitive parts is to create a drawing with views and then save it as a template. When you start a new drawing with the template you get to select the parts for the views.
SW Explorer can be used, too.
My challenge is when I have an assembly with parts and drawings, I cannot find the part drawings in SW Explorer and change them.

Crashj 'well, not my only challenge' Johnson

 

[RawheadRex]

Another alternative involving SW Explorer:

[ol][li]When it is determined that you need to create A2 and D2 copy files for A1 and D1 to a different folder using Windows Explorer.[/li]

[li]Launch SW Explorer[/li]

[li]Select File[/li]

[li]Select Open[/li]

[li]Browse to the folder location where you copied A1 and D1[/li]

[li]Select D1 and click Open[/li]

[li]In SW Explorer window RMB D1 at the top of the list[/li]

[li]Select Rename[/li]

[li]Change D1 to D2 in the field next to the word "To:" (Note - the filename of the currently selected item is shown in the greyed out field immediately above, next to the word "Rename:&quot[/li]

[li]Click "Find Now"[/li]

[li]Click "Apply"[/li]

[li]The drawing name is changed[/li]

[li]Repeat steps 3-11 to rename A1 to A2[/li][/ol]

There is an FAQ posted here on Eng-Tips related to SW Explorer that explains this a bit more in case anyone's interested.

For what it's worth, I find the results of the SW Explorer method of managing and updating references more predictable as in the past (pre-SW99) dealing with them inside SW had negative consequences for us at the company I was with at the time. Having said that though I do think it's lame that a SP change would hose functionality that's been present for a few releases.

One last question; mncad when you say "haven't found a way in SW Explorer to do it," do you mean you've never managed references in SW Explorer before or that there's something with the files that prevents changing/updating references?



Chris Gervais
Sr. Mechanical Designer
Lytron Corp.

 

[powder99]

Solidworks sp5.1 fixes the reference issue

 

[dogarila]

If powder99 is right then they DID make another SP (5.1 to fix what they messed up in 5.0). Thanx SolidWorks.

Powder99, have you used SP5.1? I have reinstalled SW2003 and SPs up to 4.0 and, after what happened to SP5 I am really afraid to install this new 5.1 service pack.

 

[JNR]

Just browsing through, so I know this is a bit late, but I noticed in nmcad's Nov 18 post that he calims file created in SP5.0 are fine. Just a thought - if you saved the files with SP5.0, would it fix the problem?

I was - and he did. So at least I didn't get coal.....
OK, OK, It's a reference to my holiday sig. "Be naughty - Save Santa a trip..."

 

[powder99]

I have had no problems so far. The list of fixes for the 5.1 service pack are outlined below. Fix 191763 refers to the issue in this thread.

SolidWorks 2003 SP 5.1
The following problems/enhancements have been addressed in SolidWorks 2003 SP 5.1: SPR # Description

190314 Center mark for circular hole through cylindrical body is not located properly.

***191763 Open drawing and change references to find a file in a different directory not working.

192275 Component Names are not properly updated in the assembly FeatureManager when a Save As operation is performed on a part in the assembly.

192434 Curve driven pattern will not consistently generate in SolidWorks 2003 SP5.0. Pattern may generate after several forced rebuilds.