Current state of Model Based Definition 1

[KENAT]

There have been several threads both here and in other forums on use of MBD (Model Based Dimensioning). When I'd previously looked at it I'd decided it would be more effort than it would be worth for most of our stuff, however, have implemented it on some castings and moldings.

We're being pushed to decrease development time cycles and my boss wants to look at MBD as a way of achieving this.

So how many people are doing MBD and have any major developments in this field come along since it was last discussed in depth?

I'm especially interested in those out side of the 'managed supply chain' of Aerospace/Defense and Automotive where it seems to have been achieved largely by the OEM's dictating what CAD system will be used and using their leverage to enforce this on their suppliers.

We are a smaller/independent player in the technology field who outsource all our machining etc. with only assembly done in house (even some of this is outsourced) and I'm wondering how other smaller players have dealt with it. Do you:

1. Only deal with suppliers with the same (or at least compatible) CAD/CAM system(s) so that tolerances etc. in the model are carried across?
2. Use a lightweight format and does it correctly handle MBD.?
3. Use hybrid drawing/model and if so how do you handle Tolerancing of features not explicitly defined on the drawing?
4. Have extensive "rules of use" in addition to/in place of the above or just rely on ASME Y14.41 or equivalent?

I have a copy of 14.41 and looked through it a while back but I’m not completely familiar with it.

thread1103-182896
thread730-184173
thread1103-182500
thread730-221206

Are all more or less relevant.

Thanks.



KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[fcsuper]

Models are generally considered basic except where tolerances are added. To fully define a part, you'll still need a GD&T scheme, often supplemented by traditionally dimensioning and tolerancing where needed. The difference is that this now has to be done within the model itself.

Additionally, any information that would've appeared on the drawings also now has to appear within the model itself. So, shortcutting the drawing step doesn't mean you get to not bother with all the information you would've included on the drawing. It just means all of that now needs to appear in the model.

With that said, ASME Y14.41 supposedly standardizes this effort. In my opinion (and yes I've read it and "own" a copy), it is drasically lacking right now.

If you do go MBD, just make sure everyone understands that the model is now the drawing and that means it will need to be as actually detailed as the drawing would've been.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[fcsuper]

Now, to address your 4 questions:

1. Only deal with suppliers with the same (or at least compatible) CAD/CAM system(s) so that tolerances etc. in the model are carried across?

A: In my opinion, this is not practical unless you own your suppliers. The variety of packages and versions for each package increases each year. It is good to analyze what is common in your industry, but that's not the end of this.

2. Use a lightweight format and does it correctly handle MBD.?

A: Don't know. This sounds like this question is particular to one particular 3D CAD application.

3. Use hybrid drawing/model and if so how do you handle Tolerancing of features not explicitly defined on the drawing?

A: My company does this. We still drive critically from the drawing, and use the model as the completion of the part definition. I've seen some companies callout a general profile tol based on the model for all surfaces not defined by the drawing. I've seen others simply use the model as part of the direct specification (model is not basic, but to be measured from directly with a previously established traditional tol)

4. Have extensive "rules of use" in addition to/in place of the above or just rely on ASME Y14.41 or equivalent?

A: Given my own opinion about Y14.41, I would suggest that your additional "rules of use" would have to be extentive indeed.


These are just my opinions...take them only as far as you can throw me.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[SDETERS]

1. We have a wide base of suppliers that own all kinds of different 3D software so we usually transfer the drawings in PDf and the Model in STEP and Or Parasolid format. Not many Suppliers use I-Deas anymore ):

2?

3.We call out all critical dimensions with applicaple tolerances and GD&t. We attach the following Block to our Raw Material Drawings. See attached

Thanks

 

[MechNorth]

I've seen several efforts at moving to a model based enterprise, and all have had issues.

There fortunately are well accepted neutral model formats (particularly popular are STEP and Parasolid), but they are "dumb" solids; i.e. no parametrics and no imbedded data. These are ok with CAM packages that look at the model surface, but don't consider the math behind the surfacing. This isn't the most efficient method when doing complex surfacing though, so a compatible CAM package that can use your native CAD model format is better in those situations.

From what I've seen so far, none of the CAM packages recognize the GD&T data whether annotated or imbedded into the model. That's probably because the CAD packages do a rather poor job of imbedding the GD&T into the model in the first place ... tried it ... don't like it.

What I've found works best under the situations I've been involved in is a hybrid system. Send the supplier a neutral format (Parasolid is my preference for comparatively simple geometries, but STEP works better with complex surfacing) to program their CAM packages with, and an annotated GD&T model file that they can read the annotations from. There are supposed to be some CMM packages out there that can read the imbedded GD&T data from the models of certain CAD packages, but I've not seen proof of this when challenged. What I've seen usually happen is that the GD&T is read from the print or model by a CMM pogrammer, then manually applied to the model again in the CMM software. Rather cumbersome, and prone to transcription errors.

Keep in mind that Y14.41 was written so that the CAD/CAM/CMM software developers could have a common starting point and set of functional requirements. Also, Y14.41 doesn't just apply to CAD data, but essentially defines PDM (product data management) structure and requirements. Now that Y14.5-2009 is released, the Y14.41 committee will be starting on the next revision. NOW is the time for anyone with comments & suggestions for Y14.41 to post them to ASME for consideration.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

MechNorth

"and an annotated GD&T model file that they can read the annotations from"

What do you mean by this? Are you sending both a step/parasolid type 'dumb' model and a lightweight file type, something like JT, that supposedly carries across MBD annotation etc? Why not just the JT type file?

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[ctopher]

Isn't MBD solely to replace drawings, not to be used for CAM?

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08; CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[MechNorth]

Kenat,
I've sent e-drawings with the GD&T annotations on the model, and SolidWorks files which can be viewed with a viewer program but can't be used otherwise without the SW program. I haven't tried a 3-D PDF, but I recall someone telling me that they'd had success with it for sending "dumb" annotated models.

I would send the native annotated CAD model if the supplier could use it directly, but they can't always.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[MechNorth]

Ctopher,
I don't know if there is an "official" definition of MBD. I take it to mean that the model is the basis of the design rather than a print. As a result, the model can be used directly for manufacturing and inspection. Most of the automated (CNC) shops that I've dealt with have been switching over to model-based CAM and CMM programming; those shops range in size from two machine operators to several dozen or more. Manual shops often go back to generating a drawing themselves if they receive a model ... of course GD&T isn't usually much of a consideration for them anyway.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[ewh]

I may be mistaken, but NX offers embedded GD&T which can be read by Valisys CMM software, as well as by NX CAM.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ctopher]

I did a search here at my company. MBD files are also used for CAM and include all GD&T definitions. They are the same as if they are a regular drawing.
On some programs, a separate file is used for CAM from the MBD file.
When a file is imported from another company that uses a different 3D CAD application, they have to follow certain guidelines and be pre-approved how those files are presented. I don't think they follow their own guidelines because I never had to be pre-approved in the past at other companies.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08; CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[MechNorth]

I believe you're right re NX & Valisys tolerance analysis package, wasn't aware that they had a CMM controller capability now too. Up to NX2, there was supposed to be full compatibility between the two, but we could never get it to work; the imbedding of GD&T into the model was cumbersome and we couldn't seem to get it right, so we never did get that functionality going back then. I always held out hope that by buying & integrating Valisys, UG would get things to work together. No idea of the CAM side.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

So a few more questions on the sending 2 model types (completely dumb generic format without annotation, not so generic format/viewer only capable with annotation).

Did this pose configuration control issues?

How did the annotated model formats cope with 'set views' which my CAD system at least does with it MBD annotation? This is where 'views' are created in the model with certain annotation on them, snapping to the 'view' orients the model to that view & turns on the annotation in that view.

How do you deal with non dimensional notes & general tolerances?

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[MechNorth]

Good questions.
No problems with configuration control as our manifestations (model, drawing, CAM, etc.) followed a master-model methodology; each reflected the model at that revision level. We actually found it easier to keep track of changes within the entire system because some software can track & ping changes on the master model to all subscribed users such as programming.

We didn't use set views in the model. From what I understand of the software, it's a selectable functionality that can be activated / deactivated as needed or preferred. Personally, I prefer to just rotate the model to see what's what. Per Y14.41, you are supposed to be able to activate and deactivate annotation planes also, so that you can remove the noise when you're looking for something.

In NX2 at least, we could imbed an overall surface profile as a general tolerance. Individual controls on featues overrode the general tolerance. We didn't have luck with the imbedded tolerances, so we went the annotation route instead, and put the general surface profile and all notes on designated (& named) annotation planes.

Note that imbedding and annotating are different beasts, and the two may not necessarily agree depending on how you do things.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

Thanks all for the answers, especially the detail from Matt, Jim & SDETERS To me, in my simplistic little world...

It seems that if you're going to have to send 2 different file formats, one for the base geometry and one for the 'annotation' then why not just stick with the hybrid drawing model combo. This is what we've done on some castings/moldings and at least one complex machined part.

Given the way the MBD annotation is added separately to creating the model features and other factors it doesn't seem much if any extra effort to create the (partial) drawing. Also then all information is laid out in a single 'orientation' without needing to manipulate the model and can be sent in a format like PDF that is already in common use.

If you use some kind of ‘unless otherwise stated’ default tolerance, be it surface profile with model basic (what we did) or some kind of +- to then where you get benefit is in not having to add individual dimensions/tolerances to features covered by this tol and potentially hence not needing to create as many drawing views etc to be able to show these. This is a potentially massive benefit for complex surfaced features such as are fairly common in aerospace/defense & automotive or even commercial moldings/castings.

However, where’s the benefit in many machined or even sheet metal parts? In many cases a single default tolerance that covers most features isn’t practical.

Also will having a ‘default’ tolerance cause even less attention to be paid to Tolerancing than already happens with a typical title block tolerance?

Also, if you go the default surface profile route, while I don’t believe it’s backed up by the standard, many imply this as having increased inspection implications or somehow being more complex etc. – does it lead to higher cost? I know we have to be careful of this line of thought or we end up throwing out a lot of GD & T

Most of our stuff at present the drawing is the master, however we do routinely supply step or other 'dumb' models in addition (as reference) to the drawing to help with CAM/CNC programming.

My boss is thinking of making simple parts MBD only, but to me it’s the complex parts that potentially benefit most from MBD.

Sorry for the long, in places rant like, post.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[ewh]

Jim,
Valisys still may not work as intended with NX; we had it in the budget when a new QA manager was hired. They decided not to spend the money on it, and have me compare point clouds to models to verify their data instead. ;-( The demo was quite impressive, though.
KENAT,
I think it will be awhile before MBD really takes off and meets its full potential. In the meantime, we do as many and use the hybrid method, only we state that the model is the master instead of the drawing. Most of out parts are created from lofted surfaces, and those are the features we usually consider most important. We currently send out neutral model files and jpegs, though are looking into using "lightweight" files in the future. It's like herding cats though to get a concensus around here.


"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

Thanks ewh,

The config control issues on the 'jpegs' scares me, again I'd rather have a partial drawing.

Maybe I was unclear, on the few items we have used MBD we make the model the master where applicable. It's on the parts where the drawing is complete but we send a step for info that the model is 'reference only'.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[ewh]

We consider the jpegs to be the same as any other drawing copy, and as long as we keep track of what we send out, problems are few. The trouble starts when a PO gets issued with unreleased drawings/models.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[MechNorth]

Kenat, all I can do is empathize. I'm not convinced that there is a good system in place anywhere for this, despite what PLM, PDM, CAD, CAM and Inspection software vendors claim. None of them are integrated unless they are under the same ownership. What works moderately well with one system crashes on another. I have to study Y14.41, but I'm hoping that with the next revision we'll fix some things and tighten up some loopholes.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[DesignBiz]

KENAT,
It seems as if you have had a fair amount of input as to how to handle the MBD. I might add that we use the hybrid method for the most part as you have proposed. The model is sent in “STEP” format along with PDF of a partial drawing. The drawing is used to dimension all holes and any exceptions to our general profile of a surface note. In addition all datums are defined on the drawing. As others have mentioned, attempts to imbed the GD&T into the model has presented more problems at this time than it is worth.
Even if the part is a simple machining or formed part, a partial drawing is useful for hole callouts and datum definition.


DesignBiz

"Quality is in the details"