Interview with Steve Lapic from Brentwood Ind.

Steve Lapic works as a CAD admin for the Water & Wastewater Group of Brentwood Industries. They design water clarification and biological systems for the water and wastewater industry around the world. The products they make fit into customers large tanks that are used to clean the water. The group has about 60 employees. For their work they use SolidWorks, AutoCAD and SolidWorks PDM Professional. All combined they probably have on the order of 80 licenses.

They are a project-based company.

He reached out to me via e-mail after he read my post about The Evolution of a Numbering scheme. He gave me some good advice on configuration management and also agreed to make an interview to share his system. Following is a short summary of the e-mails we exchanged. So, here it goes, enjoy!


I checked your website and I found a very nice video of the Polychem system that your company makes. If I understand correctly, when a customer orders a Polychem system like this, your company has to customize it so that it fits the customers’ needs (tank dimensions, etc.). And because of that you treat each installation as a separate project and not as a product, am I right?

Yes, every tank is different and not just in size but some have walls with recesses or protrusions that affect our designs. Many of our products can be used in any tank based on use of tank and not size. Other components must be made unique based on size of the tank. Because most facilities have multiple tanks with different sizes and uses, we need to treat this as a project to make sure we keep everything straight.

The video shows the components of the tank. If you watch it you can imagine the tank being wider would affect some components and if it was longer, we would have different quantities of other components but it would also affect the motor that moves everything since there is more components to move. Depending on the component, they may last 2 - 30 years before they have to be replaced or the system has to be replaced. 

Do you manufacture the product at your company or do you outsource?

We outsource all components. Most of the injection molded components are done with another division with in Brentwood. And there is some light assembly done at this facility.


How do you organize your CAD data in folders? Do you keep all the CAD data in one main folder that is divided in subfolders or do you keep the CAD data in folders of the specific project?

Our folder structure is set up in two top level folders for our CAD work. One is for projects and the other is for components.

The project folder is then broken down to particular project and the template that creates it also creates 55 sub-folders with 12 CAD and Office files prepopulated with variable information.

The component folder is broken down to types of components and possibly even further as needed. For instance, we have a folder called plates and that is all the further it needed to go but then we also have a folder labeled sprockets. Inside that we have a folder called NH78 Sprocket and another called NH78 Sprocket Assembly. For the most part the folder plays little in how the engineers work. When they need to make a new component, they do a search to see if one already exists or if there is something similar. If similar they usually create a new configuration of the model and get the similar drawing, copy it to the same folder with a new config name and go from there.

Another thing about the PDM, if you use a good standard description process then searching for parts based on their description while ignoring the number is the way to go.


You mentioned that you are using a non-significant numbering scheme and that you use the same part on multiple projects?

Yes, we are using an 8-digit non-significant scheme. We call them our 10 million numbers. These numbers are sequential and are generally in no particular order. To the right of the 8-digits number (family number) we have a 3-digits dash number for numbering of configurations.


Can you explain how you use configurations?

We try to keep all similar components within one family number and then use configurations to manage the differences.

Sometimes we will use new family numbers for a significant difference that will have multiple configurations. For instance, I mentioned the sprocket. We have a unique family of numbers for the different number of teeth so we have a different number for the 40 tooth sprockets, 32 tooth, 23 tooth, 17 tooth, etc. The configurations would be for different bore sizes, key sizes, split sprockets, English or metric hardware, etc.

One more example: if I needed a 316 stainless steel plate with a certain size and certain hole pattern and searching, I found one that is almost exactly what I needed but uses 304 stainless steel. Let’s say its number is 10001234-032. I would copy that config to the new one (let’s say it is 10001234-067) and change the material. I would open the -032 drawing and save it as the -067 and link it to the correct config. The drawing would automatically update to the new information. Our drawing title blocks are all property driven so the differences would automatically update with the new material, description, weight, etc.

If possible, we want to reuse component designs so multiple facilities may have the same component.

How do you decide when to make a new part with a new family number and when to make a new configuration? Do you have a rule for this?

We don’t have any hard-fast rules for this. If the part doesn’t look like it “fits” with the old ones then we make a new number for it.

For instance, if we had a tube that had a single diameter and thickness but many different lengths with the same pattern of holes but different locations, these would all be one number with different configurations. If we had one with a different diameter, we probably would give it a different number since everyone is used to this number being the one diameter.

Do you ever make a multi-part drawing or do you always keep each configuration on a separate drawing?

Normally, each part has its own drawing. But there are times that we have need of some weldments that do not use other released parts. For these we create virtual components with all of the necessary information contained on the weldment drawing.

Have you ever considered making a single drawing for all your dash numbers and adding a design table to show the different values for each dimension?

They had done this in the past (10+ years ago) but we use 8.5x11 and 11x17 paper and big charts with many configurations are not practical so we don’t use them at all.

Do all your parts and assemblies get a dash number, even if they only have one configuration (-001)?

Everything starts with a -001 even if there is only one at the moment.


How does your revision scheme look like?

Generally, we use a two-digit numeric revision scheme for everything. Within engineering we also use an additional alpha revision scheme.

The difference is when a drawing is released it uses the numeric scheme but while the drawing is in process and it passes out of a state that allows a change to the drawing then there will be an increase in the alpha revision.

This means that if a drafter passes a drawing on to a checker it would be at revision A. The checker has permissions to make changes (normally to fix typos and such) but when he sends it on it would be at revision B. If there is a change needed then it would go back to the drafter who would send on a revision C to the checker and then he would send on a revision D. If no further change is needed then it would be released at revision 01 (for some reason we start at 01 and not 00). If there is a need for a revision after release it would then go to the drafter would make the change and send it on to be checked at revision E. And so forth and so on...

Do you also revision control the parts or only the drawings?

Drawings are released, not models.

While models follow along with the drawings and can be released, we have too many models that new configurations are being added to before the drawings are released. For this reason, we find the version control that is built in good enough for understanding the parts history.

How do you decide if you make a revision or create a new part?

We use the rule that if the change affects form, fit, or function you need a new part number. Many of our parts are used on multiple projects and we don’t want to make a change so that the part no longer fits an existing or old project. Our customers call up and order parts 20 years later to replace their old part and expect it to fit. So, no changes that affect form, fit, or function.

With that in mind if I had a component that would fit perfectly but I wanted to move a hole I would just make a new part because I would know that if I made a change the part would not fit when a facility ordered a replacement part. On the other hand, if I designed a new component and released but shortly afterwards, I noticed that I had to make a change to a hole location I would check to see if it is being used on any new projects and if it wasn’t, I would then make the revision.

There are also other reasons to make a change that would be acceptable and would not affect it if it was used as a replacement part. The change could be a coating specification for example.

Also, we use PDM so we actually have a check box that gets checked off once the parts interchangeability has been confirmed.

Interesting, I really like this idea with the check box. Can you tell me how exactly this works?

Inside PDM we have a check off on our file card stating that any changes did will not affect existing projects and we have a condition in our workflow that won’t allow it to proceed until that box is checked.

In the transition from Released to Revising states I have an action to set the Revision Verification variable to NO. When the drawing is transitioned between the Revising and the Review Change states there is a condition that Revision Verification variable must equal YES. This makes a simple little loop going. When you first create it the variable defaults to NO and stays that way even after it is taken out of release but after it has been revised it needs to be YES and it will stay that way through release of the revision. Once it is pulled out of Release again for a revision it will go back to NO until it is ready to be checked again.

If someone copies an existing released revised drawing and checks it in then the Revision Verification variable would be YES. So, I put an action when a new drawing is sent to checking that variable’s value is set to NO.

We didn’t actually have this check off box until about 5 years ago. I would like to think that everyone did this before then but now you must have that box checked before the model/drawing can be changed.

Can every engineer decide on whether the part is interchangeable? Or does only a specific person get to decide on whether the part gets a new number or just a revision?

We leave it up to the engineer to decide if it is a revision or if it needs a new number (or configuration). If they are not sure they will talk to me or each other. Sometimes, but rarely, do we need to change how they decided.

Usually only new engineers will ask once or twice.  Also, all drawings, revised or new, do have to be approved before release just like everywhere else and hopefully any issues would be caught then.  I think our process has enough checks to minimize accidental release of the incorrect information in this case.


When the project is completed, what kind of files does the customer get (STEP, PDF, edraw...)?

No CAD files are sent to the customer. We only supply pdf files for maintenance and ordering of spare parts.

What about files for manufacturing?

The only file we send out is a dxf file of the nameplate since it has the logo on it and the nameplate is engraved. We do not send out STEP files. Only pdfs of the drawings.

Does this mean that the manufacturer needs to make the CAM code based only on the drawings?

Yes, but since the configurations are so similar, they can take a previous CAM file and just edit a few dimensions.


I think Steve’s company has a simple but still advanced system. It gives them the ability to make changes quickly and also the ability to reuse parts on multiple projects. Because of the check-box Steve has included in PDM, the system makes it harder for engineers to mess up other projects.

Using a non-significant numbering scheme gives them the ability to leverage the PDM systems number generator, which means less work for the engineer.

I find it interesting that as an ETO (engineer to order) company they use configurations and dash numbers. In my country this kind of companies usually decide on a one-configuration system.

As Steve said, they only manage revisions for drawings and each part gets its own drawing. Companies usually use configurations and dash numbers to make multi-part drawings with a design table to show dimensions of the more or less same parts (family of parts). This kind of drawings are very often used by product-based companies to prevent engineers from making and revisioning more or less the same drawings. I think in Steve’s company it is rarely the case that a change would affect multiple projects. So, they have simplified their system with single-part drawings. When a new configuration is needed, they just add it to the model, copy a similar drawing and point to the new configuration. If a change is actually needed on multiple configurations, like for instance a coating change, the CAD model is corrected and the drawings update automatically. So, there is no need for manual corrections.

Because Steve’s company uses two major revision schemes, they can easily see if the drawing has been released or not. This way they don’t need another database field showing the status of the drawing. So, less info to manage is a good thing.

Being a project-based company, they don’t have very strict rules for interchangeability checking and I think this is OK until every engineer gets a good basic training that helps them decide on whether or not a change is interchangeable.

If the company would ever decide to start tracking products by serial number and not project number, they would probably need to give more attention to the interchangeability rules!


I would like to thank Steve again for taking the time to share his system with me and the simpleCADstandards community! As a thank-you for his contribution he will be among the first to receive a simpleCADstandards customized gift.

Would you like to share your system with our community and receive a special gift? Drop me a line via LinkedIn or directly on and let me know…

About the Author

Barbara Jerin

Is the creator of this blog and author of the majority of blog posts.

Comments 3

  1. Hello Barbara,

    Steve said that they use an 8-digit (family) number followed by a 3-digit dash number for numbering of configurations. From his explanation of the configurations follows that the configuration number is a part of the part number. So both the family number plus the configuration number form the part ID of non-interchangeable parts. The configuration number is not the revision of the part. Only their drawings get revision indicators. So far so good.

    Because of this I am a little bit confused about the answer to the question: “Can every engineer decide on whether the part is interchangeable? Or … on whether the part gets a new number or just a revision?”
    Steve answered: “We leave it up to the engineer to decide if it is a configuration or if it needs a new number.”
    This is not the answer to the question (part ID vs. revision). Or does it mean that they call (and use) the configuration number as “revison”, what would be wrong with regard to Steve’s explanation of configurations, see above.
    What is meant by “needs a new number”? Which number?

    Best regards,

    1. Post

      Hi Jörg,

      Thank you for this explanation. I see what you mean. I will check with Steve again, to clear this up.

    2. Post

      Hi Jörg,
      I have corrected the section where the mistake was and I added some explanation to it.
      It was a misunderstanding.
      Thank you for noticing.

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