Generic modeling question

[dtharrett]

Running NX 7.5 with teamcenter integration. I have a question regarding the modeling of metric holes.

Is there a standard out there that dictates or suggests whether we should model to the nominal or the basic size?

For example, when modeling a 12mm hole with G7 tolerance the basic size is 12mm but nominal is 12.015mm

The reason I ask is because we have been modeling to the basic size and machine shops have been complaining because they like to cut to the model. I would like to respond with "you need to look at the toleranced drawing" and also reference some sort of standard.

On the flip size, you guys might come back with a standard that is contradictory to our modeling practice

 

[JohnRBaker]

If these are clearance holes for bolts, are you creating them based on the intended fastener size or are you creating a hole at a specific diameter?

On the Hole Feature dialog you have the option of creating a Hole based on several different criteria including creating a 'Screw Clearance Hole' where you select size of the screw and then based on the tolerance selected, the actual diameter of the hole will be determined by the system.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[dtharrett]

These would be for things loike dowel holes or spefic holes for items other than screws. Basically holes that are not presently intended for the NX hole feature....

 

[dtharrett]

Now that I think about it, I would use the hole wizard. But the original question still applies (nominal vs basic size) and is there a standard for this?

 

[looslib]

A lot depends on how the shop is producing the hole. If it is being burned or punched, then I tend to model them to the median dimension. If the hole is being drilled, reamed or machined, I would go for the nominal. Tapped holes would be to the tap drill size adjusted to the shops standard procedures.

Your 12mm g7 hole if being drilled or reamed, I would model at 12 since the NC programmer would be specifying the tool callout and the NC program only cares about the center point dimension.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[loki3000]

you dimension it to the basic size and include the fit tolerance. for example (diameter)12 g7. if there is a need to, you also include the fit table where you have the upper and lower boundary for all included fits.

 

[dtharrett]

loki3000,
Today we are modeling to the basic size but with no fit tolerance in the model. Is there a way to add the fit tolerance to the model and are there any industry standards that I can reference?
Thanks!

 

[loki3000]

you add a tolerance to the drawing. it might be possible on the model too, lookup "model based definition" on google.

 

[dtharrett]

Loki3000,
My questions are related to modeling (not drafting). If modeling to the basic dimension is the way to go, can this be support by any industry standard? We are designing machines/fixtures/mechanisms for what it's worth...

 

[looslib]

The only modeling standard that may have anything in it is ASME Y14.41 - Product Definition Data Set Practices - Digital.

Not sure why you need a standard to define how to create a model of your own design. Design intent and form, fit and function to your application shouyld be the drivers.

Basic dimensioning is just that, drawing related dimensioning to convey the design intent to others through a 2D drawing. Weather a hole is dimensioned with GD&T basic location or +/- location doesn't change the intent of the design.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[Walterke]

Basic dimensioning is just that, drawing related dimensioning to convey the design intent to others through a 2D drawing. Weather a hole is dimensioned with GD&T basic location or +/- location doesn't change the intent of the design.

It does change how the shop handles it.

If you need something lasered and you can provide a dxf to your suppliers, you may have less trouble if they don't have to adjust every single hole in it to make it fit it's specific tolerance.

Having worked as a laser programmer, I can, unfortunately for me at the time, say that most, if not all, drawings came in with nominal drawing, and we had to adjust to the specific tolerance ourselves.

I'm guessing the short answer to dtharrett 's original question is: No, there's no standard

NX 7.5
Teamcenter 8

 

[looslib]

The only adjustment you need to make to a nominla designed part for cutting with a laser should be the kerf. Most CNC software generation packages can handle that without you having to change the original data.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[DaSalo]

I'm going to weigh in on the side of modeling to the MEAN size. In your example "nominal" size would be the same as the basic size : 12. "Nominal" just means the NAME of the feature. In this case the hole is NAMED "12G7". The limits of size for a "12G7" hole are 12.006-12.024 making the MEAN size 12.015. The nominal size "12" is nothing more than a name. Modeling a 12G7 hole at 12mm just makes no practical sense since your model would be out of tolerance and in no way representative of what you actually want. Even the "drill bit" argument that looslib makes really doesn't apply here because with a drilled hole the nominal size would presumably still be in tolerance or that size drill bit couldn't be selected. With many fit callouts the nominal size is actually out of tolerance and just makes no sense for any purpose other than to direct you to the appropriate row in the fit table.

The my preferred practice is to give size limits and then the fit name in parenthesis for reference: 12.024-12.006 (12G7)

That all said, an argument could be made the other way based on the ASME standard:

----------
Models and 2D drawings that are intended for product definition should not be dimensioned in a way that specifies or gives preference to any particular manufacturing method:

ASMEY14.5-2009 1.4(e) : "The drawing should define a part without specifying manufacturing methods."

I don't have a copy of Y14.41 handy but I'm sure the intent there is the same.

If a manufacturer elects to use a particular programming process that depends on the model features being modeled at something other than basic size then it is their responsibility to create a manufacturing model that is appropriate to their methods. This is a manufacturing requirement, not a product definition requirement.
------------

I don't find this second argument particularly convincing or practical but I can see some kind of an opening there to make it. I think that in the majority of situations modeling to something other than the mean just invites confusion and drives costs up.





NX 7.5.4.4, NX 8.0(Evaluating)
Tecnomatix Quality 8.0.1.3

 

[dtharrett]

Perhapse I used the wrong terminology when I stated Nominal vs. Basic. What I meant, as noted above, was MEAN VS. BASIC.

One of the problems here is that some engineers are modeling basic and some are modeling by the mean. Some models have a mix of both. Either way the drawing gets dimensioned the same but the model geometry causes issues for the guys that cut to the model. Obviously we need a standard here.

I was trying to get to an industry standard that we could adopt as our standard here. I have a portion (pages 1-10) of ASME y14.41 but did not see anything however page 11 suposedly has info regarding the model requirements.

Either way, there have been some good arguments for both methods posted here.. Thanks

 

[DaSalo]

The guiding principle that I use is that I model what I really want. For example:

I just designed a gage the other day for checking the profile of an airfoil shape. It is a simple guillotine-type gage consisting of two plates, each with half of the profile. When the plates are fully closed around the part the part must not contact anywhere on the plates. If you can see light all around it passes. For this to work the plates must be cut to the maximum profile size plus a few .0001's so you can actually see light around a part that is right at MMC. This gage will function best if it is exactly MMC +.0002. MMC +.0001 would be acceptable and MMC +.001 is the high limit. I modeled it at MMC +.0002 because that is really what I want and then applied a +.0008/-.0001 tolerance.

Now the guy running the wire EDM machine probably isn't going to like that very much and is going to want a profile that is right at the mean (median? I think median is probably the better term) so that he can maximize his tolerance. In this case I don't care what he wants. My job is product definition and by modeling that gage as I did I defined my "ideal" product. I will then make a separate file with the profile modeled at the median size for manufacturing purposes if asked for it.

NX 7.5.4.4, NX 8.0(Evaluating)
Tecnomatix Quality 8.0.1.3

 

[dtharrett]

DaSalo,
Interesting point(s). I am currious how you would model a 12mm (nominal)dowel and it's corresponding press and slip fit holes. All three features at basic or meadian values?

 

[DaSalo]

Almost all of our work is done in inches so I'll tell you what I would do for a .500 nominal hardened steel dowel and slip and press fit holes in a 4140 PHT steel plate. I would do something different if it was a stainless dowel going into an aluminum plate or some other combination.

Dowel: Modeled at .500. Tolerance: +.0003/-.0000. Since this is a standard, purchased component if I were to give the tolerance on the print it would only be in the description field in the BOM.

Press fit hole: Modeled at .500. Tolerance: +/- .0002. This is what a new to slightly used HSS reamer will cut in .4140 PHT under normal conditions. Really this is a transition fit but I know that standard dowels will be +.0002 - +.0003 99% of the time and the reamers we use will cut +/- .0001 of nominal 99% of the time. So 99% of the time I'm going to get .0001-.0004 press, which is what I want, and the tiny percentage of times that I get .0001-.0002 clearance or .0005 press isn't going to hurt anything.

Slip fit hole: Modeled at .5005. Tolerance +/- .0002. This makes it clear that this is intentionally a slip fit hole and should be cut with a .0005 oversize reamer (or bored). 99% of the time I'm going to get .0001-.0004 clearance which is enough to allow assembly and disassembly in a blind hole without venting and still locate accurately enough for most purposes.


NX 7.5.4.4, NX 8.0(Evaluating)
Tecnomatix Quality 8.0.1.3