Profile control vs. Size and Location + possible refinement

[prdave00]

I have a part with 3 holes arranged to provide various amounts of offset to position pins and maintain parallelism with respect to one another. Up until now the responsible engineer has relied on linear dimensions to control location without giving much thought to controlling orientation (parallelism) as shown on the first page of the attached.

A new print was presented to me for review with an attempt made to use a profile tolerance. I had a good notion of what he wanted to accomplish so I dialed in the drawing to make it more presentable. It's the 2nd page of the attached. I've 90% convinced my self that I need a secondary datum and am leaning toward the central plane based on the .400" width or maybe one of the other holes. Any thoughts?

Actually my bigger question is whether profile control is the best strategy? I'd be more inclined to rely first on the tolerance of size and location (projected or not) as my controls and then refine with orientation (parallelism) as needed as shown on the 3rd page.

Either method in my mind would communicate the same funcional requirements, but is there anything else to consider? Is one easier to inspect than the other using a CMM for example?

 

[ctopher]

Curious...Any reason why the part would not have datums A and B on surfaces instead of the hole?

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[prdave00]

I've gone back and forth over this in my head. I always strive to add enough datums to stabilize the part, but in this case the only truly important feature is the hole in the 1st position (i.e. furthest from the handle) and then the other holes should be located and oriented with respect to that first hole. Therefore I agree with the hole as the primary datum. In my no-profile scenario, I wanted to be explicit that the series of holes should fall in a row (for aesthetic reasons). I was tempted to do this on the profile scenario too but wanted to see if excluding it would pass the red face test. The bottom face (opposite the direction the handle extension) could serve as either B or C (if a tertiary is needed), but the truth is that its orientation (perpendicularity) isn't very important and the controls of the tolerance of size control is sufficient. But does movement up and down the hole really need to be arrested for inspection?

 

[ctopher]

Without seeing the mating parts, I would go with 'method 2b' or 'original'.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[fsincox]

Can the two intersecting holes benifit from MMC? Does the part mount on a face as primary?
Frank

 

[prdave00]

The holes act as guides. For example, we have a pin plunged into a substrate and want to offset a second pin by a specific offset while maintaining parallelism. The tool is grasped by the handle and slid over the existing pin. Then a second pin is inserted into one of the other 2 holes and the is driven into place with a mallet. The perpendicular bottom face may or may not directly contact the substrate's surface. To reflect function I ruled out this face as the primary datum.

The larger the hole (whether controlled by a size or profile tolerance), the more un-parallel the two pins might be which is why I specified LMC in the positional tolerance. In other words, as the hole shrinks the better the parallelism (in theory). With that said, I would say that MMC works against me. Does this make sense?

 

[PeterStock]

As the hole shrinks the more material there is, thus MMC should be what you use. For a pin, the larger the pin, the more material, MMC is at the max dim. For a hole, the smaller the hole, the more material, MMC is at the min dim.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[Belanger]

Always be careful with profile, because it can control several qualities at the same time. What I mean is that profile as used on these holes controls size, form, orientation, and location -- do you really want all four of those qualities to be held to .003 (or .006, whichever page you go with)?

Also keep in mind some of the rules about profile: Profile tolerances must be applied to a true profile, so you have to have a basic dimension for the diameter of the three holes; you can't have them be .098 +/- .003. And profile can't use the MMC modifier, since by defintion a surface has no such thing as a maximum material condition.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[prdave00]

As the hole increases in diameter (moves to LMC) there is more slop and therefore the position (in terms of controlling orientation) needs to be tighter. As the hole shrinks (moves to MMC) there is less slop permissible so the size of the holes plays a more dominant role in limiting the amount of un-parallelism, right? This was the rational for the LMC modifier. Am I not thinking this thru correctly?

A full analysis on what tolerances are needed for the desired function has not been done by the responsible engineer, so consider the values as placeholders for now. He originally specified a profile of .003 but I assumed he really meant twice that which is why I increased it to .006". The impetus for making a change in the first place was to loosen tolerances. Prior to this exercise the distance between holes was +/-.001" and the supplier couldn't hold that nor was that offset accuracy needed. Obviously the enginner was inadvertantly proposing a tighter tolerance with the .003" profile Since the print was being revised anyway, It was decided to explore adding orientational control.

 

[PeterStock]

To insure assembly you use MMC on both sides. As the parts move away from MMC the tolerance needed to insure assembly gets larger. If your requirement is something else, you need to figure out which way, if any, the tolerance can be loosened. You may be better off at RFS. LMC I have seen used mostly for controlling wall thicknesses. On one occasion, I used zero at LMC to insure that an o-ring would not get cut when two parts were assembled.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[PeterStock]

You state that one of the holes has a pin pressed into it. You may need to use a projected tolerance zone.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[prdave00]

Peter: All holes provide for a slip fit with the pin at MMC. The only time I've ever used LMC is to control wall thickness so this might be a first that I've ever proposed LMC for something else. I may just do as you propose and suggest a RFS for this feature. I don't see it making fabrication or inspection that much harder. I've also considered a projected tolerance zone to make sure the second pin doesn't run into the first pin (at least if the 2 intersecting holes are being used), but its consideration is moot if a profile tolerance in used.

J-P: The last page where all 3 holes are assigned a +/- tolerance was from what my colleague proposed. His dimensioning scheme also suggested that these should be controlled a a pattern and not individually. I was going to propose my method 2b once I convinced myself that a profile tolerance is the way to go (which is now losing) and once he determined what he really wants from the design.