Creating a new "start part" 1

[walkersea]

I'm very new to NX3, and need to know if what I am about to propose is a good method or not.

If I create a "start part" for our usual components - e.g. a model that contains the correct datum planes, attributes, etc and then also have the drafting sheet set up with the company border, and populated with the attributes from the model. I'll store this in a read only area and then whenever a new part is created, the "start part" file is opened and saved as the correct part number.

There will only be three users initially, so no PDM system. There is a standardised system for the part numbers, and the model and detail drawing have the same part number. We don't do large assemblies, so I can't see disadvantages of doing it this way.

Anyone out there got any comments? I've seen a few threads relating to GRIP - no idea if this means I'll have to learn to program or not.

Regards.

 

[Shadowspawn]

Walkersea,
First and formost, you will certainly want/need seperate model and drawing files. This will afford you more flexibility in setting up your seperate seed parts for models and drawings, as well as keeping the assemblies from becoming unruly. I know you said that you only have small assemblies, but the file sizes will get out of hand quickly having everything in the same file and you WILL feel the performance hit. Besides, how will you detail your assemblies? Shouldn't you maintain the same basic file structure as the piece parts (ergo: master model concept)?
Secondly, as far as grip goes, grip is very useful and easy to learn for file management and drafting duties. Very handy to know (at least for me), but I can't say that you 'have to' learn grip... given the maturity of grip and the advancement of UG in general, grip probably isn't the language to put your energies into. UFUNC/OpenAPI or VB may be more beneficial in the long run...
There are others on the board that can probably answer your questions better, so hopefully it won't be long until we hear from them. Until then, I what I put forth helps.

SS

 

[ewh]

We use a system similar to Shadowspawns, that is having separate seed files for drawings and for models.
The drawing seed files contain the drawing formats and all of the attributes used in the formats, as well as layer catagories set to our standard.
The model seed files contain fewer attributes and all of the primary modeling datums, along with the layer catagories.

 

[Shadowspawn]

EWH,
By "all the primary modeling datums", you mean a datum csys, right?

SS

 

[ewh]

No, I mean datum planes and axis, which are based on the absolute csys.

 

[walkersea]

Thanks for these comments.

Sooooo, where do I find out about the Master Model concept? Reading the help file I think I understand the idea, but the practicalities of it are less certain.

The way I see it is that at part level the model & the drawing and any other documentation will have to have a unique part number - our current numbering system doesn't accommodate this. Do all the NX3 users really have part numbers that contain the type of data it contains? The help file suggests DWGxxx for the drawing assemblies, NCxxx for tool paths, etc.

As we don't have a PDM, how are the interactions between the model and drawing maintained? To work on a drawing, won't you need the model available in the working directory? If one user is working on the drawing, and another user on the model, how does the model change get reflected on the drawing?

 

[Shadowspawn]

EWH,
So why not use a datum csys? A datum CSYS is simply the 3 primary datum planes (xy,yz,xz), the 3 axis (x,y,z), a point, and a std csys ...all defined in 1 feature instead of the 6 seperate features as you describe. Also, there's no way to accidently move a primary datum plane without moving the rest of the datum csys. We've had instances of folks moving a primary datum in a file and essentially hosing the part...
Our seed parts don't contain any datums (although our modeling standards call for them...but I won't go there right now, tis too political) but the first thing I always do is add a datum csys at absolute. Everything else can be built off this datum csys...
I've found no disadvantages as of yet, and have found numerous advantages... so I was just wondering what other folks use and why.

SS

 

[ewh]

Shadowspawn,
Thanks for the heads up! Our methods are legacy for the most part, and it seems like a good time to revisit and update them. The datum csys will be the first change.

 

[wmalan]

Shadowspawn,

What the others have said about a seperate drawing file from the master model file is the most common. That said, in my industry (aerospace) several of the companys are now using a true master model setup. There is no drawing file.

The part is defined by it's actual and GD&T assigned attributes in the model file. The model file only has a view of the part in drafting with a note to reference the master model for dimensions. Boeing calls it Model Based Definition File (MDF). Northrope has the same thing. It is also done in Catia. Interesting is that Boeing only uses a Powerpoint picture of the model for initial bidding purposes. That's so their buyers have easy access to bid the parts out without having to us UG.

Shops that produce MDF parts get a copy of the part file and are required to interogate the model file for dimentions. Given much aerospace work involves complex loft data, it really works well. The down side is certified vendors are required to have UG to produce the part.

That is just one other scenario of file management.

--
Bill

 

[mjcole]

Good Tips Shadowspawn,

I'm not sure about NX3 but on NX2 you have to check off a box during CSYS creation called create components in order to get the Planes Axes and origin Points to be created.

Also another good thing about the CSYS with components is that even though it shows up as one feature, you can set the display for the AXES PLANES and CSYS display to separate Layers if you are used to having layers and categories just for AXES or PLANES.

One annoying thing about the CSYS feature is that the datums do not get resized automatically if you change the part size. There is a workaround to this IF you make a Block feature and suppress and unsupress the CSYS it will size itself to the block size.

Michael

 

[ewh]

We have also experienced MDF through Boeing. It seems to be based in part on ASME Y14.41. Once the part structure is understood, it is a better way to document a model. I am uncertain how they go about controlling the releases, revisions, etc, though.

 

[cowski]

walkersea,

The master model for the drawing basically means that you have a 1 part assembly that you generate drawing views with. Our company does not have PDM so we basically do what UG suggests; if the model is 12345.prt then the drawing is 12345_dwg.prt. This way we can easily see which file is the drawing and they show up next to each other in the directory. The 'master model method' means that one person may be changing the model while someone else is working on the drawing. In practice it is very rare that we have both files being modified at the same time, but when it happens and the model file is saved you just save the drawing file close it and reopen it and update the drawing views (then proceed to fix any of the drafting annotations that have lost associativity due to the model edits).

Depending on your load options, the files do not have to be in the same directory (or even on the same drive for that matter). My current load options are set to look first in my local hard drive (work in progress area), if it does not find the file there it looks in the network drive where part files are kept. As I change what project I am working on I will update the load options to look in that project's directory first rather than searching the entire network drive.

 

[wmalan]

Oops, my comments about MDF part files were in response to "walkersea" not Shadowspawn... not that could not be interesting to him as well. <g>

--
Bill

 

[wmalan]

ewh,

Regarding revisions with MDF: The files we got from Boeing would be something like 4G11558-1_nc for the origional. The new rev would be 4G11558-1_a. Pretty simple for us vendors really. The down side is we have to create documentation for folks on the floor for inprocess inspection which would have to be rev controled at our end as well. I personally prefer MDF being in aerospace. I program to the customers model, not a translation.

--
Bill

 

[Shadowspawn]

Wmalan,
Tis ok...no harm, no foul. I myself am greatly interested in the MDF process, as I feel that the paper drawing is largely a reflection of methodologies not keeping up with the business need or technology. While I don't think we'll be getting rid of the paper any time soon, I do think that the electronic files should be the document of record versus the paper print.
Where I work, someone took a minute or two to evaluate the use of 'smart models' and the general consensus was that they were too complex for the users and in-house processes as well as the need to get all the vendors on board with being able to effectively utilize the UG file.
I don't think I should name the company I work for, but we are in aerospace albiet not an airframer. Those guys are our direct customers... ;-) Suffice it to say that we do a ton of 1-2 part special order stuff and getting all the various casting and machine shops on UG is totally unrealistic.
Now if you have any suggestions for "cheap" software package that can fully read a UG file...

SS

 

[sewy]

Hi Shadowspawn ,
I would like to join others to thank you for this unobtrusive but very useful advice.Even if I work with Nx2 since his beginning, I have never remarked this tool. So, many thanks again.
P.S.

 

[sewy]

For your question, Solidworks of appropriate version can reads UG parts even with parameters (but not so reliable). What I know, it is not possible vice versa.

 

[abeschneider]

Shadowspawn,
Question about your CSYS tip: Do you know of a way to WAVE link a CSYS from one part into another? When I try it out, I can only WAVE the component planes of the CSYS, not the whole CSYS.

 

[Shadowspawn]

Abeschneider,
Hmmm....never tried to wave link a datum csys since I've never seen a need. I think each part should have it's own datum csys to build on, and not relying on a different part. I can see a need for wavelinking geometry (sketches or curves) and bodies (castings into a machining file), but I can't think of a reason to wavelink a csys.
If your looking for a point of reference for assembling, such as passing parts back and forth with a customer, I'd suggest placing a regular csys in a reference set to represent the point of reference.
I'll look into it a bit further soon...

SS

 

[abeschneider]

Shadowspawn,
You guessed it - I wanted to use the CSYS as a common reference point for assembly. In the past, I've WAVE'd the 3 fixed datums from a master part as the common point of reference. I'm not sure I follow your suggestion about placing a regular CSYS in a reference set - can you explain?
Thanks.