Master Model Approach...Does it make sense in my case?

[asrura1]

We are using NX9, no TC.

I was going through settings in Customer Default and noticed that there is something called Master Model. Out of curiosity, I did some research. It turns out that it is actually the recommended method for CAD. I worked with Solidworks and Solid Edge before and Master Model how those software worked.

This is a bit surprising to me because when I started my job using NX, I thought that having the 3D model and 2D drawing within the same file was so cool. It removes the headache of trying to locate the Part file when opening the Drawing file. All the companies I worked for are small companies, with their own home grown way of doing things. So, sometimes files get moved around or change directory...basically they were "liberal" and "flexible" about file management.

Now, I read quite a bit on Master Model and it seems to me that it benefits mostly large projects where different people might work on the same thing, or when revisions are made frequently. For example, one guy does the 3D model and another guy make 2D drawings for it. But for my company, our projects are not so complicated, only 20~40 components for each product. And each person works on one product/project so there is no sharing of files or work. The manufacturing processes we use are casting and machining (lathe mostly). The casting and machining are done by contractors.

In our case, would it make sense to use the Master Model approach? We almost never make revisions if the products work right. When I think about using Master Model approach for my projects, it seems to me that it's more complicated and troublesome than it needs to be. Am I wrong? Is there some advantages I am not seeing for using Master Model approach in my case?

For assembly, however, I do use the Master Model approach.

 

[JohnRBaker]

Since you're already using Master Model when making Drawings of an Assembly, why not be consistent? Remember "Consistency is a virtue in itself."

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[asrura1]

I use Master Model approach to assemble components. We almost never make drawings for assemblies, except for exploded parts drawings.

So, I take it that in this case, it's not particular advantageous or disadvantageous to use Master Model approach?

I am still debating. I have a tendency to follow "best practices" but it is just so convenient to have the 3D Model and 2D drawing within the same file.

 

[JohnRBaker]

And while we will continue to support both approaches, Master Model and embedded Drawings, in terms of future enhancments, when it comes time to decide the scope of a project, if it will be too complex or require significant additional resources to do both, the default will be to support Master Model first, and perhaps exclusively.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

Do you have a layering standard in place? If not, you'll probably need one. One of the main advantages of the master model method is being able to use reference sets to filter out the construction geometry. If the model and drawing are in the same file, "layer visibility in view" becomes the primary means of filtering the geometry from the drawing views.

The answer may also depend on your business rules. To make a long story short, at a previous employer we used the save date on the model file as a check in the process. We could modify the drawing file as needed, add views, add/remove dimensions, change tolerances, add/remove notes, etc. and still know when the last change to the model occurred.

www.nxjournaling.com

 

[asrura1]

@John
Thank you for your insight into the future direction of NX. I guess the move to Master Model approach is inevitable, even lower-end CAD package are using it.

Is there like a standard or a guide on managing files using Master Model Approach?

The biggest issue that I face is probably dealing with a part at different production stages. For example, I am design a body frame and I design it with the dimensions of a finished product in mind. Then when it is ready to make mold to die-cast it, I need to remove some features and change the dimensions of certain features. In the past, I just copy the file of finished product and then do the die-cast dimensions. But as you can see, if I change something that is shared between finished product and die-casted product, I need to update both files. From what I read, Master Model approach can deal with this but I am not sure HOW it is dealt with.

Thinking back to my Solidworks days, our file management is pretty much non-existent so I never really learned how to do it properly.

I can see myself at this company for quite a while. They give us a lot of freedom and autonomy in product design, and not much office politics which is a BIG plus in my book. So, I would like to have a system/procedure in place for all my future projects and better my skills.

 

[asrura1]

@cowski,

Thank you for your reply. No, we don't use a layering standard when doing 3D models. I think the main reason is because our components are simple.

But I would like to know more about this layering standard. From what you described, I noticed the words "reference sets" and "construction geometry".

I have seen command in NX called "reference sets". Not exactly sure what it is but I will check out NX help.

But for "construction geometry", do you mean like sketch elements that are used as aids to draw a 2D sketch to form 3D features? Like center lines or lines turned into reference?

"To make a long story short, at a previous employer we used the save date on the model file as a check in the process. We could modify the drawing file as needed, add views, add/remove dimensions, change tolerances, add/remove notes, etc. and still know when the last change to the model occurred."

So, for this method, the same model file is being updated but you create new drawings for each revision and each revision is named with the save date of the model? If model is updated, the drawings created prior to the update becomes "out of date" in NX. If someone accidentally "updated" the "out of date" drawings, how would you fix that? Or, it's not fixable? Or...you can "lock" the out of date drawing to prevent any changes (i think I read something like this somewhere)?

 

[Xwheelguy]

As far file management goes, if you move forward with master model usage, I'd strongly suggest coming up with a naming convention to ease in quickly identifying what kind of files you're looking at, as all NX files have the same (.prt) extension - which will not indicate anything to the user (is it a dwg, a model, an assembly, a casting, a machined part, etc.).

My previous job dealt with a casting and then a machined or finished - we needed both models for specific reasons. It ended up being easiest to develop the finished part first as 2D profiles, then for the added material/stock on the casting we simply offset said profiles to start the casting. The finish profiles were used as "cutters" to remove material away from the casting model. I'm sure as you try different approaches, you'll find ways to improve your design process. You may also consider getting some training onsite that's customized for your company's product and processes - let the trainer assist you in coming up with your modeling practices. It's a bit more expensive, but I feel you get more bang for your buck that way.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

In...

Customer Defaults -> Gateway -> General -> File New

...you set-up either prefixes or suffixes, as well as the separator character used, for automatic naming of various types of part files.

Granted, when you actually go to enter the name when you hit the 'Save' button for the first time or the 'Save As' button, it's still up to you as to whether you retain of the 'automatic' portion of the file name, but at least it provides a mechanism to get you started in the right direction as long as you're careful and consistent.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

But I would like to know more about this layering standard.

There is no universal layering standard, and with recent versions of NX you can largely ignore layers. However, if you move toward keeping the model and drawing in the same part file, you may want to reserve layers for certain objects (i.e. the title block should be on its own layer). The reason is: all the entities in your file will show up in drawing views (datums, sketches, sheet bodies, etc), most of which you won't want in the drawing view. When using the master model method, these "extras" are filtered out by using a reference set. When the drawing is in the same file, you will need to use "layer visible in view" to filter them out, therefore you will need to start paying attention to what object(s) go on what layer. I'd suggest something simple such as finished model on layer 1, drawing objects on layer 256, use the other layers as you see fit. Then in the drawing views you can specify only layer 1 to be shown and only the finished model will show up.

In my previous post I mentioned the "save date on the model file", by which I meant the "last modified date" as reported by Windows. We did not add the date as part of the file name. All of our released parts had a simple 5 digit part number; drawings had _dwg appended after the part number.

www.nxjournaling.com