3D Modeling Best Practice 2

[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. 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?

 

[SteveMartin]

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.

 

[KENAT]

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

thread1103-239768 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 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[drawoh]

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

 

[bbook1]

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.

 

[KENAT]

?

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 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[bbook1]

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

 

[ewh]

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." - [small]Robert Hunter[/small]

 

[handleman]

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)

 

[drawoh]

...

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

 

[aardvarkdw]

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

 

[NomLaser]

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.

 

[ajack1]

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.

 

[KENAT]

bbook1, all's well, confusion reigns.

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[ewh]

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." - [small]Robert Hunter[/small]

 

[fcsuper]

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

 

[MechEng2005]

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

 

[ajack1]

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.

 

[ewh]

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." - [small]Robert Hunter[/small]

 

[KENAT]

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

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

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​