×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

3D Modeling Best Practice
2

3D Modeling Best Practice

3D Modeling Best Practice

(OP)
If you are creating a 3D model that is going to be used to create a CNC program, how should the model be drawn in regards to the tolernacing.  For example, if a diameter is 33mm +0.3/-0.0 how would you draw the diameter?  Would you make it 33mm or dimension it at the center of the tolerance?

RE: 3D Modeling Best Practice

I don't know if this matches a standard, but my general modelling method is almost everything to the center of tolerance bands.  The only routine exception (which isn't really routine, since I don't have much cause to model them in my current employ) is metric hole/shaft basis tolerance scheme, which I would normally leave at the basic size.

RE: 3D Modeling Best Practice

There have been threads asking or at least discussing this before, take a look and try to find them.

thread1103-239768: Current state of Model Based Definition will give you a starter and links to several others.

I don't recal there being a consensus.  Quite a few model it on the mean value as I recall to allow tolerance either side but this is not universal and even then leaves the question of what to do for things like drill tolerances or true Max/Min cases or even standard shaft fits etc.

So, assuming a male feature I'd probably model 33.15.  For a female feature it would depend, I'd be tempted to model it on the nominal drill size that would be used to creae the hole if aplicable though for a hole this big that may not be relevant.

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?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: 3D Modeling Best Practice

bbook1,

   My models are used to generate fabrication drawings which are issued to jobbing shops.  I model most things to nominal dimension, and I set tolerances on the drawings to get the fits that I actually want.  

   The next time I generate a 3D model that will go straight out to a fabricator, I will model everything to the median dimension, i.e. the average of the maximum and minimum acceptable dimension.  My one and only experience with fabricating from the model is with rapid prototyping, and I am fairly certain that they never looked at my drawings.

   Talk to your fabricator.  You need to understand how they are going to program their process.  Our machinists ask for DXF copies of our drawings.  Are your's going to examine the tolerances on your drawing or model?  Are there any standards they understand?

               JHG

RE: 3D Modeling Best Practice

(OP)
KENAT,
Thanks for your post, you might want to reread number 2 of http://www.eng-tips.com/faqs.cfm?fid=376 that you posted above.

Is there a standard that addresses this debate?

Drawoh,
We are trying to move towards CAD to CUT with our machine shop and trying to decide what makes the most sense when using a 3D model as opposed to a dimensioned drawing.  I have used several Rapid Prototype CNC companies, whenever I send them something I always use the median.  Part of this comes from an arguement that I have had with my CAD guy, he always uses the base dimension and several times we have had parts made that use either -/- or +/+ tolerancing so the models are always wrong when we have them made since the dimension will never be the base value.

RE: 3D Modeling Best Practice

?

You have a funny way of trying to get help.  

Those last 3 links are part of my signature.  If you want to start throwing rule compliance around how about you try #1.  Or if I was so off topic just red flag my post.

While I can't remember which one(s), and especially given your response am not inclined to dig deeper, I'm pretty sure some of the other threads listed in the thread I linked did address this topic.  If not one of them then somewhere else.  I was not trying to broaden this into general MBD debate, merely pointing out that this specific topic has come up in the more general debate.

14.41 is the MBD modelling standard but doesn't cover this type of thing.

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?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: 3D Modeling Best Practice

(OP)
KENAT,

Sorry, the dividing line separting your signature from your post makes it look like another post.  I appologize if I offended you, I didn't mean to.  I appreciate your help.  I did quite a bit of google searching before I came to this forum, the problem is defining what you are looking for in a way that gives relavent info.  I was about to buy 14.41, I'm glad that you mentioned that it doesn't address this.  With all of the Aerospace, Automotive guys doing everything primarily in 3D, I figured there would be more definition of this thing out there rather than opinion.

Again, sorry if I PO'd you.

Brian

RE: 3D Modeling Best Practice

It may be opinion, but it is usually well-reasoned opinion.
That said, we generally model at the median value.

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

RE: 3D Modeling Best Practice

Talk to the CNC operator.  They should know what they want in order to give you the best chance of an in-spec part.

They may actually ask you to model closer to MMC, especially if the model is a complex one that will add up to lots of time.  You can always take more off, can't really add it back on.

-handleman, CSWP (The new, easy test)

RE: 3D Modeling Best Practice

Quote (bbook1):


...

Drawoh,
We are trying to move towards CAD to CUT with our machine shop and trying to decide what makes the most sense when using a 3D model as opposed to a dimensioned drawing.

...

   Make sure you provide your vendors with some media that controls tolerances.  

   This is why I like drawings.  I can very quickly generate a 3D model off of a fabrication drawing, unless the drawing is a mess.  If I were a vendor with the ability to fabricate from 3D models, I would seriously consider making my own models my way from the vendor's drawings, whenever possible.  This will work very well with orthogonal, machined parts.   It will not work at all if you are designing Marilyn Monroe shaped electric toothbrushes.

   I agree with your CAD guy about using base dimensions, however, you have to get your parts fabricated and inspected.  Your drawings and models have to be readable by the end-user.

               JHG

RE: 3D Modeling Best Practice

Speaking as an NC Programmer, I typically get models that are nominal and it is up to me to adjust my offsets to compensate for machine/tool tolerance, drawing tolerances, vibration, etc... It is fairly common for me to cut a part slightly heavy in areas that have flush cuts or similar features and let the operator hand work the mismatch.

It would be easier to have the parts modeled to the best size for machining and to just drive the contour and not have to worry about offsets but more often than not I have to tweak things anyway. Furthermore the chances of the engineer knowing the best size within the tolerance is, lets face it slim. That is why the company pays me to figure this stuff out. If you are going to spend a bunch of time modeling the part to the machining tolerances, you might as well program it as well, and you have better things to do with your time and the company's money.

As a draftsman, I would without a doubt model the part to the nominal dimension that is on the print. Do not model the part differently as this just creates confusion.

I have always tried to tolerance and design parts so that the median is nominal but I know in some circumstances this does not match design intent and you have to use -/- or +/+ tolerances.

The bottom line is, concentrate on communicating exactly what you want and what you will accept and the programmer/operator will do their job and give it to you.

David

RE: 3D Modeling Best Practice

As Kenat said, it has been discussed to death.  I'll throw in my 2 cents.  From an Engineering point it makes sense to model the part to the fits that you want to use.  This way when you go back you can easily see what fit you used even if you have double negative or double positive tolerances.  

From the Programmer's point of view, it's a pain to have to shift surfaces or features so that you hit the double (positive or negative) tolerance.  Either way you need to make the decision if you NC programmers are capable or not.  At one company that I worked for I had to model to the mean and use +/- tolerances because they didn't have the time to figure out +/+ or -/- tolerances.

RE: 3D Modeling Best Practice

This has been discussed many times and there does not seem to be a one size fits all solution.

If all work is done in house on the same CAD/Cam system life is slightly easier as most systems have some sort of feature recognition and by using "internal standards" face colour, slight tweaks on sizes etc things can be sorted. If however you just intend to send the model to someone the other side of the world in a neutral format it is highly unlikely this will work.

As for rapid prototyping, well if you mean SLS or SLA then you will get as near as possible what your model, many companies that provide this service will just take your model and convert it to a .stl file or similar, this in itself losses some accuracy. As for features like tapped holes, I am not aware of any CAD system that actually creates a "tapped" hole, however it is debatable if a threaded hole will be of a suitable standard anyway.

If you wish to cut directly to a model you will need to set internal standards, there will be problems along the way but the benefits are also huge, especially on complex 3D shapes.
 

RE: 3D Modeling Best Practice

ajack1,
Just an FYI, there are CAD systems which can model threads, it just isn't used very often.

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

RE: 3D Modeling Best Practice

Just a reminder, if the drawing is elimenated, the information on the drawing needs to be moved to the model itself, which means the work still has to go into dimensioning the model correctly.  General profile notes help, but they don't solve particular critical areas well.

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: 3D Modeling Best Practice

In general, I'd go with nominal dimensions unless there was a reason to make it something else. My thought is that if the "rule" were to make everything MMC, including raw materials, then should I model a 3/8" x 1 1/2" HR steel bar as 0.387 x 1 17/32? And the cold rolled version might be .379" thick.

For items you know are going to be machined, I would tend towards going with nominal to indicate design intent. However, in some cases it may be worth while to indicate things differently. If for example a box needed to hold at least a certain volume, and it didn't matter much if it was bigger, then I might think about using the minimum values with a positive tolerance.


-- MechEng2005

RE: 3D Modeling Best Practice

Ewh, sorry I did not mean to imply that threads cannot be modelled; they can be on any reasonable CAD system, what I meant was if you put a standard tapped hole in, no CAD system (I am aware of) will actually create a true thread. It will however create the appearance of a threaded hole in any 2D drawings and be recognised as such by a compatible CAM system.

RE: 3D Modeling Best Practice

I don't know, not having actually checked their dimensions.  You may be right, but they do look accurate.

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

RE: 3D Modeling Best Practice

I think ajack means that by default, most CAD systems have some kind of 'simplified representation' which may or may not show up in the model as 'appearing' to be a thread, will show up in a 2D drawing as a thread you can call out but when turned into iges or step will lose that info.  At least on the systems I've worked if you wanted the actual thread modelled you had to take extra/non standard steps.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: 3D Modeling Best Practice

It is just a toggle on NX, but as I posted, I have never verified their accuracy.

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

RE: 3D Modeling Best Practice

I know the McMaster Carr models/drawing have the thread modeled (as opposed to just a graphical representation). It's really irritating and can dramatically increase file sizes and slow performance. I have no idea what software they use to generate their models/drawings though.

-- MechEng2005

RE: 3D Modeling Best Practice

Most of the McMaster hardware that I've seen/used does not have a thread modeled, just something that looks like one at quick glance.  I agree that it's a pain, because it's both slow and wrong.  I usually delete out all the faux-threads and put in a cosmetic thread if I'm using one of those models for something.  It takes longer up front, but doesn't annoy me every time I use the model.
 

RE: 3D Modeling Best Practice

This is a bit off topic but I've got a bunch of fastener models from McMaster that have threads and that I'm debating tidying up.

On topic, the more I think about it the more I think you'll have to talk to your machine shop(s) and ask what's best for them then come up with your own procedure.

For general machining I can see 'mean' perhaps being best but for some process I'd suspect otherwise.  For instance traditional drill tolerances allow for the fact that holes tend to drill oversize.  To me it still makes sense to model the nominal drill size, rather than the mean which would be typically a couple of thou' bigger and wouldnt' match a standard drill size.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: 3D Modeling Best Practice

Quote (MechEng2005):

I have no idea what software they use to generate their models/drawings though.
I'm pretty sure it's SolidWorks. It's the only native parametric filetype they offer.

Quote (bbook1):

If you are creating a 3D model that is going to be used to create a CNC program, how should the model be drawn in regards to the tolernacing.
It really comes down to discussing this with the person who's doing the CAM programming. That's the most reliable way to ensure that any offsets and adjustments will produce a part that is within tolerance. Sometimes that means creating a special version of the model, but most often, the CAM technician handles it based on the drawing's tolerances.

RE: 3D Modeling Best Practice

Some CAD systems let you have your cake & eat it too.  Pro/E will let you have a dimension like 5+0/-.2 which normally will measure 5.0.  However, you can go into to the part setup/dimension bounds and change any or all dimensions to upper, middle, lower or nominal.  Changing the above dimension to "middle" will regen to 4.9 while the drawing will still say 5+0/-.2.  

Similarly, you can have a max dimension like R0.3 max regen to measure 0.15 by setting the upper tol to 0, the lower tol equal to the nominal and regening to the middle.

This has saved me tons of work by always having the model geometry at nominal but the drawing can show the fully associative parametric asymmetric model dimension.

RE: 3D Modeling Best Practice

Autodesk Inventor allows you to apply tolerances to the model dimensions (a bit cumbersome the last time I used it but effective), these dimensions could then be toggled to Nominal, Mean, Upper, or Lower tolerance size and would allow you to check fits in the assembly.

Unfortunately this information is not carried over when parts are saved out as neutral format files and I don't know if there are many CAM programs that read native Inventor files.  

  

David

RE: 3D Modeling Best Practice

That is the problem, as I stated many systems (I do not have a full working knowledge of every CAD system on the market) will create some kind of feature recognition that works with a compatible CAM system, however again to the best of my knowledge this goes out of the window when used on a CAM system that is not directly compatible and you use .iges .stp or whatever neutral files.

RE: 3D Modeling Best Practice

dgallup;

"........However, you can go into to the part setup/dimension bounds and change any or all dimensions to upper, middle, lower or nominal.........."

Thanks, thats something I had not realized about Pro/E and just became part of my "best practices".

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services
www.infotechpr.net

RE: 3D Modeling Best Practice

Regarding McMaster-Carr threads, they are garbage, used only for appearance sake.  If you look closely at them, they are only angled torii, nothing like a true helix.

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

RE: 3D Modeling Best Practice

Model to nominal and tolerance to standard fits (symmetric, bilateral, MAX, etc.).  Why? There are two reasons.

1) You can perform an interference check with coincident faces considered as interference.  This will allow you to quick identify, check,and update the fit of nominal interfaces.

2) NC programmers can provide an offset which will leave or take more material.  This can be implemented at any point in the code.  So if the overall size of your part is +/- .005" they'll run the cutter nominal. However, if you have a internal profile that needs +.002"/-.000 they'll run the rough nominal and run the finish pass nominal with a .001" offset.  The point is tolerances are easily programmed by a capable NC Programmer.

Be consistent and work with your vendor and they will make the parts right.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources