solidworks plays musical parts behind my back 2

[cmm]

Two parts having the same filename, stored anywhere on my computer or the company network, which may or may not be identical parts, are sometimes substituted for one another automatically by SW03SP4 without my knowledge. I do not want to change my filenaming scheme to one where every part within reach of my computer has a unique filename. Usually the parts are the same, they just reside in different assembly folders. Our ME dept has been enduring this problem for years. Is anyone else having this problem?

 

[MadMango]

Take a look at your System Options> File Locations and see if the order of the file locations are set properly. If you always store these files locally, then you might want to move that location up the search hierarchy.

Also, it's not wise to have dupicate model files in various places if you don't need them. You don't need to have copies everywhere, you can just reference the models.

MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[ctopher]

You should never have duplicate files, keep them in a central directory on your server. Having duplicates will always create headaches for you one way or another.

 

[automationbabe]

You can also select "References" upon opening an assembly and point to the components you want to open from the directory you want.

 

[cmm]

Having a "common parts folder" containing parts used in mulitple assemblies means that assembly folders cannot be self-contained. In other words, to send an assembly to someone I'll have to manually pick out which common parts are called by that assembly. And if a common part is modified or replaced at a later date (say we receive a better model of a purchase part) then all assemblies created previously that call that part will not rebuild. When I say assemblies I mean assemblies within a current project or past projects, stored on my computer or elsewhere. How do y'all deal with this?

 

[ShaggyPE]

cmm, I too am in a situation like you describe. I often work on projects in a couple of locations which do not have access to my company's server. I create folders which house an entire project. In this folder I have folders for Manufactured parts, Off the shelf, and drawings. The off the shelf parts folder contains copies of some of the standard components that are in my main hardware folder on the server. Whenever I need to update an off the shelf part, I update the one in the server and copy that over to the assy folder. This is a bit of a headache but it does make the transfer of my files to and fro easier.

P.S. I am the only one using these files so there is no worry about sharing or having others follow the system. This may not be a luxury you have.

 

[macPT]

This issue as allredy been discussed in other threds.

You must pay attention to the way SW retrieves a file.

SW allways "remember" the location of the last opened file. If, for example, you retrieve an assembly in some location with the part "part1.sldprt", save the work, and retrieve onother assembly, from another location, with another "part1.sldprt", SW remembers the location of the first file and this is the one that is actualy being edited.

To avoid that and to be certain that the files being edited are the right ones, before I open the files, I change the option File location (the first file location on the option table). This way I force SW to search this location before any other.

When I change the project, I change the first file location option again.

Regards

 

[ShaggyPE]

The solution that macPT provided seems excellent. Another practice that I always abide by when jumping to different projects is to completely close the project I was working on. This will ensure that no references are changed.

 

[MadMango]

For more info on how SW searches for referenced files, go to the SW Help index and type in "search", then look in "file locations for external references". That should give you a good understanding.

MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[JNR]

You think you have problems..... We use SmarTeam PDM so whenever you check in and out again it automatically preserves the old versions. Even so, one of our drafters was so paranoid about loosing files, he had mutliple (no, he had MULTIPLE) folders of backups on his hard-drive. He used to get all confused and think the system had lost data of not filed. Of course than only made him more paranoid and so it was a vicious circle. We only discovered what was going one when he complained that he couldn't file his drawing one day and I discovered his 80Gig disk was full!!!

Take heed of the responses already offered and never keep more than one copy of the same file on you disk.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[StarrRider]

Cmm

Your reason for avoiding a "common parts folder" is all wet. If you do need to send an assembly to someone, you do not need to manually select the common parts. Simply open the assembly and do a SaveAs to a new directory and use the button to copy all of the Referenced parts at the same time.

As for your statement about updated models, you are wrong there too. This one of the beautiful things in SW. If I have a part named Bearing, .75 - 1.25 x .5 – Omega 123 and get an updated model of the part. Then I simply delete the old part and give the new one the same name. The only problem that you are likely to face here is that some of your constraints will be screwed up. That happens because the names of the faces in the new part, depending on how it was built, may not have the same names as the faces in the old part. If you are simply adding detail to an existing part this is not an issue. If this is a new part and is widely used – then you would spend a lot of time fixing the constraints – so you might consider doing this instead.

Open both parts first, then do a where used on the old part and open each of those assemblies. Look to see which faces that are actually constrained. In the old part, rename each of those faces / planes and then save everything. Rename the same faces / planes in the new part. I know that this is not widely done but it is not difficult. After the old file is replaced, there should be no problems when the assemblies are opened again.

The reason you are having problems is that you are using identically named files. Take as an example an assembly that has 2 sub-assemblies in it and each subassembly has a different a Bearing but both files are simply named Bearing.sldprt.
If you have nothing else open in SW and open your main assembly, which bearing will be used?

I use a Common parts folder and never change my Options/File Locations. So – the first subassembly that was inserted in your main assembly will be loaded first. SW will not open your second Bearing. sldprt file because a file with that name is already open. As a result, both subassemblies will use the same bearing – which means that the second subassembly is WRONG! If you opened the other subassembly first, then the first subassembly would be WRONG!

How do you solve this? DO NOT use generic file names. EVERY file that I create has a unique file name similar to: Part Number – Description / OR / Description – Part Number. I use the first with manufactured parts and the second with purchased parts – which allows similar parts to be grouped together.

I hope this helps.

Lee

Consciousness: That annoying time between naps.

 

[JNR]

Well, I don't know about strong statements like "you are all wet". We can't possible allow manual file copying and renaming going on in our company. Too many possiblities for human error. Sorry, ain't going to happen. The FAA and our customers would go ballistic (and I think you might think twice about flying on an airplane with avionics designed in such an uncontrolled manner). The AS9100 auditor would have an absolute yit fit! Bet you are not AS9100 or even ISO 900x certified... and if you are your auditor should be fired.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[StarrRider]

I apologize for the “all wet” statement. I didn’t mean it to be an insult or in any way derogatory – and I am sorry if it was taken that way.

JNR

I been using SW without PDM since 99. As a result, I do a lot of things manually because they are simply faster and easier for me. This doesn’t mean that the approach I explained isn’t valid.

I assume that you are finding fault with the file deletion and renaming that I suggested in the second paragraph. Please forgive me; I use Windows Explorer for almost everything and that is the way I think. I am aware that many people run into trouble handling files outside of SW and I should have given the “proper” SW command instead. I rewrote it this way:
Open both models and make sure that the properties are identical. After closing the original model, do a SaveAs with the new model and select the original model so that it is replaced. The only problem that you are likely to find is that in the assemblies that used the model, some of your constraints may be screwed up. This happens because the database names for the faces in the new model may not be the same as those in the original model. If you are simply adding detail to an existing part this is not an issue, but with a completely new model it can be. If the original part was widely used – then you could spend a lot of time fixing constraints – so you might consider doing this instead.

Open both parts. Do a where used on the original model and open each of the assemblies listed. Look to see which faces are actually used to constrain the part. Change the dbase names for those faces/planes in both your part files. Since the assemblies are open, they will be updated when you are finished, so save and close the original model and all of the assemblies. Finally, do a SaveAs on the new file and select the original model. Renaming faces and planes is not widely done but it is not difficult, select the face and RMB Face Property - it probably will not have a name but you can give it one. All of the constraints should be valid when the assemblies are opened again.

Using the SaveAs in SW does exactly the same thing as that I originally described using Windows Explorer except that with the SaveAs, there will be an extra file left on your system that you will have to delete manually anyway (the unsaved new file).

I did omit one thing. All of the assemblies should be reopened after the new file is “renamed” or replaced because SW will issue a warning when the assembly is opened the next time stating that the ID of the file is not the same as the ID of the original file.

Even if you are using a PDM system, that should work. Your PDM system may question you about the “New” file when you check it back in, but so what? You replaced an old model with a new model and updated all related assemblies at the same time. I personally don’t see why an ISO 9xxx Auditor would question the methodology of how this was accomplished, providing it was done correctly. I am assuming here that the files were checked out properly and then checked back in after the changes were made.

I am not a stranger to ISO 9xxx but from your comments, I am not sure how much you actually know about those standards. ISO 9xxx only provide guidelines that a company CAN follow. They do not force a company to implement a PDM system or define how the PDM system will to operate. For a company to receive ISO 9xxx certification, it simply has to state how they will do specific things and then be able to prove that they are, in fact, operating according to those guidelines when an Auditor arrives. If they specify that you have to use leaves in the restroom, and implement a method of monitoring leaf usage, then you had better start using leaves or find another job because they will loose their certification when the Auditor arrives. At the same time, if they do not add a ridiculous specification like that then they do not have to adhere to it – and EVERY company has it’s own guidelines. It is unfortunate that in some companies, the people who write those specifications don’t communicate very well with the people who are going to have to use the system that they define. It is also unfortunate that a lot of companies start off with ISO 9001 (which does not concern Engineering) and eventually move up to ISO 9002 (which does). Having lived through the transition twice, I know that many of the 9001 processes effect how things are done in 9002 and if Engineering had been consulted originally they never would have been implemented as they were.

Finally, I too have worked in aviation. First for KC Aviation, at Love Field in Dallas TX creating STC 3 drawings for Canadair and GulfStreams. Later it was for Garrett Aviation, at Van Nuys, CA documenting Avionics. Both of those positions were using AutoCAD, not SW.

Lee

Consciousness: That annoying time between naps.

 

[DeSimulacra]

I see that this is an old thread but it best addresses the number one issue I have with SW. The ending was left hanging and still lacks a promising answer. Many of the replies are based on larger company networks; SW is based on the premise that it is user friendly for all users including people who can’t afford PDM (<- what’s that ) or a full time guru keeping up with part numbers-revisions-lost constraints.
We are a 3 man engineering team with myself the point man leading this company into 3D. I have been looking at SW’s file management for a few weeks. Looking at this thread and others it is confirmed there are issues. All of the posts helped but none are >opinion here< complete solutions for small companies.
I’m not throwing rocks because anyone good enough to help/offer solutions is a great guy/girl and it worked for them. “I am” looking for a better solution for my company.

If someone will answer the question below in the affirmative and post the solution then I will post how a rock solid “small company” solution might be found. It is one I’ve employed for years without trouble with other similar software. Not listed here to keep length of post down.
I would like to know: 1) If there is anyway to set a working directory so SW never "automatically"looks outside of that directory. 2) If #1 above is yes is it possible to change that directory easily during each session? If either answer is negative someone with clout needs to point this out to SW and incorporate these as options in the next version. “Cause” I know SW listens to us grunts (fingers crossed and breath held).

Sincerely
Mark

 

[SBaugh]

You should post this as a new question and use this thread as a reference.

Regards,

Scott Baugh, CSWP to me

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If your in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[SBaugh]

I didn't have time to answer earlier

1) No, it always uses the last saved folder (this is a Windows function) try doing the same thing in Word.

The only thing you can do to get your enhancements in is to fill out an Enhancement Request at the SW website.

Regards,

Scott Baugh, CSWP to me

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If your in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[JDavidM]

Please refer to thread559-26989

If you set up the default file folder, that seems to be the cause of many a problem. I had that same problem, but when I removed the default folder, the problems went away.