Product Structuring without PDM

[generalpatton]

Our firm has 9 seats of SWX in a couple of satellite locations. At the time we purchased SWX, we had a signicant turnover of upper management who maintained the standards and procedures. To date we haven't re-established those standards. We are operating on the company network using a Windows folder setup.

We are making a jump to have our shop floor read our solidworks files directly rather than issuing pdf's, parasolids, etc.

Without getting long-winded, using configurations appears to present a problem since each drawing does not have its own unique file to point towards.

I'd be interested to hear of any methods that worked well and methods to avoid to make the most of solidworks and allow smooth access to the shop floor.

Links, stories, ideas and horror stories are all welcome!

 

[CorBlimeyLimey]

"Dash" numbers can be used in a chart (general table or design table) in a drawing. eg. 12345-1, 12345-2)

Separate sheets in a multi-sheet drawing can also be used. Each sheet having a unique "dash" designation.

 

[drawoh]

generalpatton,

Using configurations can cause all sorts of problems if you do not think your system through carefully. What does the shop do with your drawings, and what problems are you having?

When you prepare models and drawings, you have to understand your end user requirements.

JHG

 

[MadMango]

I'd be interested to hear of any methods that worked well and methods to avoid...

First off, don't let the Shop folks have access to your original files. If you must, create a folder that they can access which contains copies of your files. That will prevent them from ruining all your work (which will happen), but also creates an additional control point that must be maintained and updated in some manner. Renaming the files with the revision level can be successful.


I'd be curious to hear the reason why a neutral file format cannot be used by the shop? By giving them "dumb models", you take away the ability for them to inadvertently change the model and make bad parts.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[CorBlimeyLimey]

I agree with MadMango ... the shop floor only need the eDrawing package to view the drawings and models. Giving them SolidWorks is asking for trouble.

 

[Gurjjeet]

If you really wanna give them the SolidWorks Acess

Intall PDM, then setup users & permissions
& then sit back & relax.

they will be able to make PDFs for themselves, which means one less thing for you to do.

We all are only looking at the data editing point of view, you will need to make sure it does not get deleted(Your company might have a back-up thing but still who wants to lose the data), so PDM is gud for that reason as well.

 

[generalpatton]

Our previous process was to produce pdf's, dxf's and parasolids from which the floor would get their information.

The new process is not yet in place but will be such that the floor will have read-only access to SWX files and would be able to directly read what information they need.

My initial thought was that we would use configs for efficiency during design/prototype phase and break out files to the proper nomenclature when released to manufacturing. That has quite a few issues to work through, however.

 

[rgrayclamps]

Hi, generalpatton:

Below are my advices:

1) Whether using a PDM or not, you need to have a quick way to find where models are used, so that when you revise them, you know impacts of the changes to other documents;

2) Use sequential non-intelligent part numebrs;

3) One model and drawing for each part/assembly (item). Stay away from configuration;

4) Setup your vault security.

Good luck!

Alex

 

[generalpatton]

First, thanks for everyone's input.

rgray,
Not sure if we could operate efficiently without configurations during the pre-released stage, especially when dealing with families of products.

Hmmm, I guess that supports the idea of breaking the configs apart when released to the shop floor. No apparent magic bullet.

 

[JMarv]

Intall PDM, then setup users & permissions

This can be done in the network environment, without using any PDM. Anyone can have read only access to the engineering files, but only authorized personel need write access to the files. At my company this is controlled by your network login/username.

If you have the extra seats of SolidWorks, it would be a better tool to use than eDrawings, provided the shop floor only has read only access to the files.

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[rgrayclamps]

Hi, generalpatton:

One model and one print per item is as efficient if not more efficient than any tabulated approaches.

In modern ERP, items need to be independent due to what is called "normalization".

Also, you need to be very careful with definition of "families of products". What is "families of product"?
Generally, it refers to similar items. But what is similarity? How do you define similarity? Where do you draw a thick line to indicate items are similar or not.

One print, one model per item is the way to go in my oppinion.

Best regards,

Alex

 

[EEnd]

The parametric nature of the native SW files poses some challenges for product specification and revision control. There is no guarantee that when the shop floor opens the model they will have the exact same model that the designer had when they saved it. That is why I prefer static representations like PDF and parasolid for conveying product specifications.

Examples in which the model can change unexpectedly:
[ul]
[li]External references to other part and assembly files. If the referenced file is different in the manufacturing context than in the design context, the dependent model can be changed without people understanding why, or even knowing that it happened.[/li]
[li]Equations. In addition to being sources of external references, it is possible to create equations which change the model at every rebuild.[/li]
[li]Configurations. There is the question about which configuration to use, which you encountered. Also design tables can be a source of equations and external references as well.[/li][/ul]

External references, equations and configurations are convenient during design, but can pose some revision control nightmares. I think there are macros to save all the configurations as separate files, equations can be disabled and external references can be broken.

If you go forward with using the SW files, your release procedure should include steps for making the model static prior to submitting them for use by the shop floor.

Eric

 

[drawoh]

...
First off, don't let the Shop folks have access to your original files.

Many years ago, I set up a document control process on a UNIX network. The files lived in their working directories. I wrote a set of shell scripts to manage ECRs, document check in, document check out, and all sorts of search tools. Everything was readable, but anything not being actively worked on was read-only. We were using AutoCAD, and we were not using XREFs.

If your files are stored read-only, the shop cannot screw anything up.

generalpatton,

Eventually, we transferred files over to a Windows filesystem, and we brought in a document control guy to administer all this. Also, we installed Mechanical Desktop, and I used it for a couple of design projects.

Mechanical Desktop and AutoCAD use the complete file path to locate XREFs. If someone reorganizes your directories (folders), all your XREFs break. If your files are stored in a directory tree you do not have complete control over, you are dead meat.

I suspect SolidWorks would be a disaster too. PDM copies all your required files out of a database, into your working directory. This is the first place SolidWorks searches for them.

A directory tree is not a robust way to store externally referenced CAD data.

JHG

 

[fcsuper]

I know this doesn't really address your question, but many if the issues you will have with a network drive system can be addressed by using a PDM. Workgroup PDM is effectively free (you may already have it if you purchased SW Profession). I would consider at least employing it. With VPN, it can be used for small multisite organziations with relative success.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[rgrayclamps]

Hi,

It is true that if your files are stored read-only, the shop cannot screw anything up. But the shop may see documents differently from the original ones. Depending on how each station's setup, you may get big surprises upon openning the documents.

When you open Solidworks documents, SW may go through more than a dozen of search mechanisms to locate referenced documents. SW documents this in "Search Routine for Referenced Documents". The same file name at different locations has different priority. SW grabs external references based on this priority.

It is not mistake-proof to view SW math data directly for production purpose.

I compeletely agree with EEnd that static representations like PDF and parasolid for conveying product specifications is a safer approach.

Good luck,

Alex

 

[generalpatton]

The floor won't use swx for opening files. Only Edrawings will be used. So using this for viewing a slddrw file is a static event, correct? Or will interpretation errors be possible?

 

[rgrayclamps]

Hi, generalpatton:

Yes, it is a static event, and a snapshot, but it does not always indicate your model was fully resolved (upto date). Interpreation errors are highly possible.

If your drawing references a standalone (i.e, no external referneces) model, it is safe. However, if the model has external references, e-drawing won't be able to indicate the model is fully resolved (presence of external reference, evaluation of equations, and etc.).

Good luck!

Alex

 

[EEnd]

You might try saving the files as eDrawings files. I have not verified this, but I suspect it will protect you from problems caused by external references, equations and design tables. You will still want to save each configuration as a separate file.

Performing a save as may seem like an extra step, but it provides significant value. A single SolidWorks file can specify multiple different parts. The save as step is where the designer says, “This is what I want built.”

Eric