Revision management 7

[Andy330hp]

Hi,
I'm part of a startup company, and we're having some questions concerning the management of our drawings.
I have some experience with Solidworks during through college (I'm a recent grad) but am not an expert. So, I can make pretty nice models, but I've never had to do much organization
Our biggest question is about the organization and creation of revisions. What kind of features does SW2003 have that can help us automate the process? Is there a way to automatically generate a revision block? Can you then reference the Rev number in the title block to the last revision in the revision block?
Once a new revision of a part is made, a subsequent revision of the assembly must also be made. Once the new part is inserted, is there a way to automatically update the parts list in the drawing to reflect this? I may be asking for a little much here, but if there isn't a way to do it now maybe these discussions will spur them into adding it to future versions!

 

[EdDanzer]

If the assembly changes because there is a part change, then it must have a part number change. For large assemblies this can take time but at least you know when a change was made if the items are serialized. If SolidWorks could understand how this worked from the parts level to the parts manual level it could be automated. I was at there office 3 times to explain how this would work, but gave up.

 

[Standing]

Several Engineers in our group insist on creating names for parts, e.g. TopPlate.sldprt. After the design is complete they want to rename the part to 634123.sldprt. They found out that they need to have the part open, the parts’ drawing open, the next assembly model open and the drawing of the assembly open. This would allow them to change all of them at once. If they did not have all drawings and models opened this created a real mess. I personally do not create non-real numbers anymore. I get a good number from Doc control before starting a part. Is renumbering (using revision in part #) a problem when renaming your parts?

Bradley

 

[sirmick]

Using revs in part number is not a problem for me because I follow my procedure. Which is to make sure that each assembly and drawing that is going to change is incremented and reved properly. However, I don't see how this would be different if a part was swapped out with one of an entirely different number.

To me its the same end result. Now, a problem occurs if your company issues drawings and doesn't want the problem of a controlled drawing with a given rev number changing and the rev number staying static. To me this is a no-no.

 

[drawoh]

Andy330hp,

Consider how your manufacturing is going to work. Someone is going to take your BOM, walk into the stock room and build a kit of parts to be assembled. Shortly afterwards, someone else will take the kit and your assembly drawing and put everything together. If every single item on your BOM is correct, then all the required parts will have been ordered, stocked and kitted. If your assembly drawing is all correct, then the item numbers will correspond to the BOM. You should have made your drawing clear enough that the assembler can identify stuff sitting in the kit. The system will be assembled and it will work.

Any part numbers in the system must point to a parts bin with the correct parts in it. The part number on the BOM must be the correct part. This all requires discipline on your part.

Suggestions:

1.) Do not apply the revision number to your part numbers.

2.) Do not modify parts.

You may revise drawings to clarify information, or to correct mistakes. In the case of mistakes, it is assumed here that the parts were fabricated correctly, and you have brought the drawings into conformance. CAD drawings routinely have missing dimensions for example.

If you want to change a part, you generate a new model, and new drawing and a new part number. Alternately, you can tabulate the drawing, adding a code to indicate the new part. The original number is still valid, and unmodified.

This is all crucial once you build a library of parts and start using stuff on several assemblies and projects. When you change the form, fit and/or function of an existing part, you are possibly screwing up an existing design.

If effect, if you organize SolidWorks correctly, you should never have to check out the solid model of a part.

At the assembly level, you should not change the form, fit and function. You can modify the assembly, but it must be forwards and backwards compatible to the existing version. You should log the revision number when you build the assembly.

JHG

 

[Andy330hp]

Thank you all very much for your input. I think I am going to be able to follow the general consensus of nondescript part numbers w/o revision information. I believe our companies past errors and manufacturing issues were becuase they were calling changes "revisions" even though parts were changing dramatically.

On a related issue: Say I change a part. And, say its p/n was number 1001. The new part is 1002. It is ver similar to 1001, so much so that I would like to reuse the drawing file for 1001 and incorporate the changes. What is the correct renaming/saving sequence to make this happen fluidly. I have messed this up and have had to fool SW by renaming files, moving things around, and basically doing what shouldn't be done (in my opinion) to get the drawing to look at the new part. I just bought Murray's book, I haven't found any info on this yet (in honesty, I'm going cover to cover and haven't even hit the drawing section yet). Thanks
Andy

 

[EdDanzer]

To make a drawing reference a different part, close the drawing, click on open drawing, click on the file you want, then click on the “References” box in the lower RH corner and change the path to the correct file and then hit “Open”

Good luck

 

[StarrRider]

Andy330Hp

The easiest (and safest) way to create a new model and drawing is to start from the drawing. Lets say that you do need to create the part 1002 from part 1001. Open the drawing for part 1001 / do a SaveAs to part 1002 / then using the RMB open the model for 1001 and do a SaveAs to 1002 there as well / Changer your Custom Properties for the new part / Save your model / Switch to the drawing and save it as well. The links in the drawing will be updated and you can make any modifications to it as needed.

The only problem with this approach is that if you have an assembly open that uses part number 1001 in it, every instance will be changed to part number 1002. To prevent this – make sure that the assembly is not open when you create your new part.

Lee

Consciousness: That annoying time between naps.

 

[rustdogbrown]

I think it would be nice if SW was "link friendly" with excel. Then all of BOM'sand other costing info could be updated automatically. New part numbers and description could be managed concurrently with drawings and revisions......the advantages are many. Let me know if you find anything!

L8R Sk8R

 

[Andy330hp]

Okay, so what about this? (sorry to keep bugging, you can tell me to go away at any time)

Currently the old drafter has left many files with different configurations. Lets say the first file, which has a descriptive name "widget.sldprt", has 3 configurations (one casting and two machining) for which I will be assigning 3 distinct part numbers. Is it okay, in your opinion, if I just leave the descriptive name for the part file? So far, we have been talking about purely sequential numeric numbering for everything, but I can't really give the one sldprt file one numeric name because it contains 3 different p/n's within. Should he have made distinct part files for each? And if so, what would be the point of having configurations in the first place?

CAD was so much easier in college when these issues didn't exist!

 

[MadMango]

If you use BOMs on your drawings, then it will look like this:

1001
1002
widget
1004

If you can live with that...

I would still assign a nonsignificant part number to your widget with 3 configs. Are the 3 configs reflecting machining operations for the part, or do the configs reflect 3 distinct parts used in different ways?

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

 

[rustdogbrown]

I would take the time to give everything a part number. Down to what is delivered by your suppliers or what comes out of the CNC, etc. Even have P/N's for the workpiece and machine time/labor time. Then construct BOM's for your finished deliverables. Tedious at first, rewarding later.

Regards

 

[Andy330hp]

The widget file's three configs:

1. Casting
2. Machined
3. Slightly different machining

In each configuration's properties, I WOULD assign part numbers. But which (if any) part number should I choose to rename the file as a whole, and why even bother if I can set up the assembly and drawing files to look at the information in the configuration properties? It's a file naming issue vs property assigning issue.

Rustdog, to clarify, are you suggesting that I take this file and split it into three seperate files, with correct part numbers for names, and eliminate the use of configurations? I was actually thinking of doing that, it has the benefit of being easy to track but the downside is that I would have a LOT of work ahead of me. I'll do whatever is necessary to make things right though

 

[automationbabe]

Andy330hp-

At my last company, we had similar models like the one you are describing. We gave it a base part number 10000-xxx and the seperate configs would be 10000-1 (config name casting), 10000-2(config name machined), etc. They shared the same drawing. Manufacturing would control the process and which sheet drawing to issue depending on the machinig process. It worked well. If a part could no longer share the base part number because form, fit and function change, then it was assigned a new number.

Your other related note: SolidWorks Explorer works well for using the drawing of similar parts.

Good luck!

 

[drawoh]

Andy330hp,

I have not had a really good chance to play with castings. I had a preliminary design going at one point, but we wound up doing it differently. Consider the following scenario.

1. I design a casting, part number 1005.

2. I machine the casting to create part number 1006.

3. I now want a modified version of the machined casting, so I create part number 1175.

Part numbers 1006 and 1175 are fabricated from part number 1005. I can implement this in SolidWorks such that the model of the casting does not get modified.

First, I create a drawing and a part model for the casting.

Second, I create a drawing and an assembly model for the machined part. I insert the casting into the assembly model. Within the assembly model, I carry out my intended machining operations. I do NOT edit the part. SolidWorks lets you remove material at the assembly level. I document all of this on the machining drawing.

Since my fabrication drawing is an assembly, I have the option of adding thread inserts and dowel pins, and using SolidWorks' BOM features to document these. Most of my fabrication drawings are attached to assembly models rather than to part models for this very reason.

Now, consider what you have done in real life. You have designed a casting for which the company has paid something like $10K in tooling. You have designed a machined part out of the casting, which may have cost a couple hundred bucks in CNC programming.

You want to modify the part. The casting is very expensive to modify, and the machining is very cheap to modify. You create a new drawing and a new assembly model. You attach the old casting part model, and generate and document your new machining procedure. The part model for the casting remains locked up in your PDM system if you have it, or else the part file remains read-only.

JHG

 

[TheTick]

to Bradley:

I noticed your earlier post about changing file names. You do not need to open all related files to change a file name. Have you fully investigated the SW Explorer? It allows one to rename files and updated all its references within a search path.

Good and evil: wrap them up and disguise it as people.

 

[Standing]

to TheTick,
We never have looked at the SolidWorks Explorer. It sounds like it would save a lot of time and renaming issues. When time permits I will look into it.
Thanks for the advice.


Bradley

 

[StarrRider]

Andy330Hp

I have to agree with Drawoh

In my last company we did something very similar with electrical control boxes that we purchased and then modified to fit our needs. The only difference was that we had a dash number filing system. There are a lot of reasons why this kind of system is desirable, but in this case, the biggest one is the ability to keep similar files together making locating a file easy.
With a control box, since it is actually an assembly, we created the box components with the same filename but a different modifying descriptor like:
123456-001 Control Box 34x48.SLDPRT
123456-001 Control Box Door 34x48.SLDPRT
The assembly that used them was
123456-001 Control Box 34x48.SLDASM
This allowed the assembly to function (door open/closed) properly. This worked because the assembly was the purchased part and the 2 internal parts would never be purchased separately.

In the modified control box assembly, we placed any cuts or holes needed and gave the part a dash numbered like
123456-002 Project 1 Control Box.SLDASM
The drawing had the same name and was normally a multi-page full-scale drawing that the machine shop used as a template.

One advantage to this was that when we needed to use the control box on another project – most of the work was already accomplished. In fact – most of the time we would simply open the drawing for the original project / save it to the next dash number (–003) / open the assembly & save it to -003 / modify the custom properties / and then make the necessary modifications.

Dash numbers are very beneficial in other ways as well. The best reason for using them that I can think of is the tabulated drawings (a design table driven parts). The problem with their usage is that there is only 1 model and drawing for a lot of parts.
Since most of us used Windows Explorer to open parts and drawings rather than SolidWorks, we needed something to differentiate these files. What we did was to change the dash numbers in the filename to x’s. We used this as a flag to state - There is something special or unusual about this file.
123456-xxx The title of the drawing was added here.SLDPRT

Please note that this still allow the sorting routine in Windows Explorer to order the files properly.

Lee

Consciousness: That annoying time between naps.

 

[TheTick]

For what it's worth to know...

Unigraphics had a built-in system for recognizing file revisions based on actual file names. It was flexible enough to accomodate nearly every conceivable naming convention. Very difficult to set up in some cases, though.

All this machinery making modern music can still be open-hearted.

 

[Andy330hp]

drawoh,
What is the difference between what you did and creating a derived part? In fact, wouldn't it be (marginally) better to create a derived part, so that it is in fact saved as a part and not as an assembly? I don't know if actually is any minute benefit in terms of the way solidworks treats the different file types...

 

[EdDanzer]

Apparently having extremely long part numbers for drawing and parts helps engineers keep things straight, but what about manufacturing, shipping, accounting, product support and the end user? If you do all the function I’ve listed above you will soon understand why a part number and drawing for each part, and in some cases each step of the processing is important. Try taking or giving an order over the phone for 10 parts with more than 8 characters, then go to inventory and pull the parts and see how this effects efficiency and accuracy.