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Current state of Model Based Definition

Current state of Model Based Definition

Current state of Model Based Definition

(OP)
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: Using 3D Model Geometry
thread730-184173: Are drawings needed anymore?
thread1103-182500: Detailing Complex Geometry
thread730-221206: I Hate Drawings!!!

Are all more or less relevant.

Thanks.



KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

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

RE: Current state of Model Based Definition

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

RE: Current state of Model Based Definition

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
 

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

(OP)
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: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

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

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

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." - Robert Hunter
 

RE: Current state of Model Based Definition

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

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

(OP)
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: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

(OP)
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: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

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." - Robert Hunter
 

RE: Current state of Model Based Definition

(OP)
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: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

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.  hammer

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

RE: Current state of Model Based Definition

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Current state of Model Based Definition

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 stpatrick2

"Quality is in the details"
 

RE: Current state of Model Based Definition

(OP)
Thanks all.  While I've gained some usefull information it seems that most of my original opinions/impressions were fairly accurate.

I spent some time last night looking at ASME Y14.41-2003 and it does seem like much (most?) of it is more about setting the standard for what the CAD packages should be able to do than with what the individiual designer should be doing.

I don't think our current primary CAD system does anywhere near all of the stuff it requires, though I'm not overly familiar with it's capabilities.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

What Cad Format DO you use.  I think Catia and I-Deas is the closest 3D modeling software that comes anywhere close to meeting the needs of ASME Y14.41-2003.  They both still have down falls But it is getting there.  I-Deas is going to NX or What was Unigraphics so hopefully in the near future there will be a 3D modeling package that will be capable of meeting these needs.

RE: Current state of Model Based Definition

(OP)
Our primary CAD system is the other Siemens/UGS offering - Solid Edge.  It has some 'PMI'(Product Manufacturing Information)  functionality with our current version (19) I'm not sure yet how much it introduces with the newer versions.  

If I understand the standard, then in many cases if you 'query' a FCF in the model, then the surface or feature it applies to is meant to 'hi-light' and vice versa.  I don't think it does this and there were a few other things I wasnt sure about.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

(OP)
I'm currently putting together a presentation on MBD to try and share my limited knowledge with management.  My attempts at verbal communication have met with no success, I'm hoping they can understand some pretty pictures and bright coloured bullet points!

On the bright side, both my boss and his boss seem to have realized we'd probably need some kind of PLM/PDM.

On the bad side my boss is already talking to potential vendors without seeming to know what MBD really means.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

(OP)
Thanks, I'll need it!

By the way, your blog came up as the first result when I googled solidworks MBD.  Good as it is I was a bit surprised there wasn't more from SW themselves.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

Uh-oh... Our IT dept did the same thing, and sent down and edict that we were to use Sharepoint for all of our file control.  "Hey, we have it, so use it" was their thinking. hammer
Of course, that went over like a lead brick when the CAD administrator (me) heard about it.  We still don't have a PDM system in place, though it is supposed to be in the 2010 budget.  This, after it had already been in the budget for 2007 and 2008.  Go figure...
At least make sure that your boss understands what is required to control relational databases before he signs off on anything.

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

RE: Current state of Model Based Definition

(OP)
Does that mean first I have to learn "what is required to control relational databases"winky smile?

We spent a bunch of time looking at PDM/PLM in 05-07 and got no where.  An aborted 'INSIGHT' implementation, which is a 'free' SE PDM that piggy backs on sharepoint, took place in late 05.  We spent much of 06 looking at what it would take to make that work or what other options were needed.  We then looked more generally at what our requirement was etc but that went real slow and we got told to pick our best guess.  Picked Teamcenter, got a quote etc. and then got told we had no money for it at end of 07.

(How'd I get a star on my own question?)

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

Because it is a good question of general interest would be my guess.

By a program that can handle "relational databases" I am refering to one that, when a part file is changed, it knows enough to report all of the files that the change affects.

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

RE: Current state of Model Based Definition

Right.
TeamCenter is out choice so far as well.

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

RE: Current state of Model Based Definition

We are currently going from Our I-Deas TDM to the teamcenter Engineering.   

RE: Current state of Model Based Definition

Quote (ctopher):

Isn't MBD solely to replace drawings, not to be used for CAM?
We have been using it for just the opposite; neutral model files for CAM and CMM use, and reduced dimension drawings for tolerancing and other annotations.  While we have the ability to annotate the models, it is fairly useless when few of our vendors can read them.

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

RE: Current state of Model Based Definition

KENAT as far as I am aware only Catia offers what you are asking for and that is still dependant on everyone in the supply chain working with it, there maybe other systems that do this but I am not aware of them. Again as far as I am aware no dumb solids can do this.

We design tooling mostly for the automotive industry, complex press tooling and moulds and have been working almost exclusively with only 3D models for a good few years. We operate a mid priced CAD/CAM system design for this market and so do most of our customers.

This type of work is fairly unique in two ways. Firstly all of our customers do their own manufacturing and understand what they are manufacturing and secondly whilst there are many complex surfaces only key areas are really tied up, for example guide pillars to guide bushes, punches to dies, dowel pins etc. Within our software there is a feature recognition system so you can apply tolerance and fit to certain items and this is recognised at the CAM stage, whilst this works well for this type of work it might not for other types.

Other "get arounds" include the use of face colour to denote certain operations or fudging sizes to denote certain criteria, the list is too long to try and explain on here. So I guess from your original post this would fall in the extensive rules of use category.

This does have plusses and minuses, you need to work very closely with chosen suppliers and have a very good working relationship with them, but it allows huge savings in terms of time and cost in getting to the market place and makes both parties "valuable" to each other.

If your bosses want to just throw quotes around the world and quote standard blah blah and pick up the cheapest, I would say they are bound to fail. If however they want to work closely with suppliers and try to solve the many problems that will arise, you can gain a significant advantage over the competition.
 

RE: Current state of Model Based Definition

(OP)
Well, my boss had his conversation with the vendor and apparantly they reckon Inventor has the most capability at the moment in terms of being able to pull the annotation from the CAD model into the CAM and work with it.

I'd seen mostly bad press, or at least not particularly encouraging, for inventor so was a bit surprised.  Anyone care to comment?

Also found out our director doesn't know the difference between a CAD model and a CAD drawing.  Awesome.

KENAT,

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RE: Current state of Model Based Definition

Hey, at least your still working, and it seems like you'll have a lot more to do to keep you busy. winky smile  

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

RE: Current state of Model Based Definition

I think The Cam package they are pulling the inventor file into is GIBBS?  Is this correct or is it a different cad Package?

 

RE: Current state of Model Based Definition

(OP)
I wasn't in on the call.  They don't just do machining, they have some design capablilities and use a bunch of different software and claimed inventor was the only one that really pulls the data through.  I was surprised and not having been in on the call still have my doubts.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Current state of Model Based Definition

Considering that there are CAM packages embedded into SolidWorks that use SolidWorks files natively, I would want to ask for an explantion about what they mean by " pulls the data through".  If you are using the application on native files natively within the editing software, there's nothing to "pull though" because its already there.

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

RE: Current state of Model Based Definition

I was wondering that, too.  It's one thing attempting to pull the data through from a differing CAD system, but quite different when using the same system for design, machining and inspection.

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

RE: Current state of Model Based Definition

(OP)
Yeah, I'd have thought if you were using an embedded or equivalent CAM package, it would pull through the data.  Like I said I wasn't on the call.

I think the phone call told my boss enough that he sees that with current technology and our place in the supply chain etc. hybrid model & drawing is probably as far as we can reasonably go.

It's just my ego that smarts from him not accepting it from me when we first spoke about it.

KENAT,

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