Position frame placement

[wojciechr]

Please see the attached file. I'm making a print with gd&t that supposed to be based on older drawing (3 top views). In my opinion though the bottom view shows the way it should be dimensioned correctly (gdt frame placement). Would you agree with me, or would you say that top views are acceptable to the asme standard too?

Thanks,
Wojciech

 

[dingy2]

I am blown away at the positional tolerances of 8 inches???? That just has to be wrong. Maybe someone thinks that is the size value - Hope not or your company is in big trouble.

Please explain.

Thanks

Dave D.

http://www.qmsi.ca

 

[wojciechr]

Oh, it's an export locomotive. The units are millimeters. Eight inch tolerance would definitely be a bit too much

Thanks,
Wojciech

 

[fsincox]

Looks like they are using position when they mean perp. I was instructed not to do that if all I really want is perp.
Looks like a typical process oriented start layout. I am not a process oriented guy, so, I would start with one bore, perp opposing faces to it, then locate second bore (possibly refine for orientation), perp it's faces to it (I have seen crankshafts where the bosses can be different lengths) then profile the stuff to the bores.

 

[Belanger]

The tip-off that it's metric is that there is a floating zero in front of the decimal point for those values that are less than 1. (That said, there is no need to take the tolerances to three decimal places.)

Your revised design is OK as far as the placement of the feature control frames goes. I notice that you doubled the tolerance that controls perpendicularity (from 0.2 to 0.4). Also, the bottom of the three frames on the right-hand hole should use the perpendicularity symbol, since that's all it does.


The old design is also OK according to the ASME standard, except for the two things that I already mentioned: the extra zeros in the feature control frames and the position tolerances of 0.2 should be perpendicularity.

I have other questions about the new design, but the placement of the frames is OK.

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

 

[flash3780]

I'd try to look at this functionally. Firstly, why are centralizing datums necessary? Does using a centerplane datum add anything to your part? Centralizing datums are difficult to inspect at RFS, and add stackup to your design if measured at MMC.

This is how I'd approach it:

I'd move datums A and B off of the stick dimensions; you may wish to add a parallelism refinement to the opposing surface.

The distance between the holes is likely your most important requirement. I would define the hole on the right as datum C (held perpendicular to A), then locate the other hole a distance away with a basic dimension and a position tolerance referencing B and C (at MMC). You may also wish to add a perpendicularity referenced to datum B as a refinement.

I'd then define the second hole as datum D. That should give you enough datums to completely define the part. From there, the exterior of the part could be defined with basic dimensions and surface profile tolerances referenced to tied back to datums A-B, C (at MMC), and D (at MMC).

 

[flash3780]

One more thing, it's often useful to add a flatness refinement to planar datum features (ex datums A and B in the above example).

Also, in the above dimensioning scheme, A parallelism refinement on the surface defining datum B relative to datum A will also hold the two surfaces in the same orientation. Not sure, but this may be another requirement of your design.

 

[MechNorth]

Similar thought to Flash, but slightly different.

First, Consider defining the two bottom surfaces as coplanar datum feature A by relating the two surfaces by means of a surface profile without a datum reference, then attaching the datum feature callout to the feature control frame.

Next,make the pattern of two holes (whether or not they are actually the same size is irrelevant) datum feature B, with a position control relating the two holes together by the principle of simultaneous requirements (same datum reference frame), and the tolerance zone specified at MMC. This establishes a centering effect which can be used to control the surrounding cast/forged features. The faces opposite to coplanar datum features A could then be located wrt datum A by means of a surface profile, or a linear-toleranced size dimension, depending on functional requirements.

Note that if you are going to use two surfaces as a compound or coplanar datum feature, then you must locate them wrt each other. The only geometric control that locates a surface is profile of a surface.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[wojciechr]

Yes, our prints are very process oriented. Your idea to constrain cast surfaces to machined features really blew my mind. Real eye opener. Not sure if I'm going to be able to push a drawing like that through our checking dep, but thank you anyway.

I changed the perpendicularity call out. Thank you.

The checker is favoring splitting and placing the horizontal (to datum E) and vertical (to datum C) position frames separatly the way it was done in the old design, because in his opinion that's easier for the "manufacturing guy" to understand.

The problem that I'm having is that it really clutters my drawing and in my opinion that makes the drawing more complicated and harder to read more that anything else.

The reason behind using casting centers as datums is centralizing the machined holes in the casting - process oriented drawing...

Thank you all for your input,
Wojciech

 

[flash3780]

I'm still of the school that drawings should be primarily function oriented (although mindful of manufacturing). The manufacturer (being an expert in manufacturing) is then free to choose how to meet the required dimensions.

That being said, in recognizing that multiple suppliers are often used for various operations (i.e. a casting vendor and a machining vendor), our parts are often broken into separate casting and machining drawings.

If I were doing it in that way, the casting drawing for a part like this would include datum targets on the round ends to simulate v-blocks (similar to Fig 4-12 of ASME Y14.8M). You'd need a second planar datum represented by three pins to tie it down in the other directions. Since castings are often irregularly shaped, we often define the surfaces with basic dimensions and profile of a surface. Most recently, we've started using a note applying a standard profile (referenced to the casting datums) to cast surfaces and referencing the supplier to the solid model (which they seem to be okay with). Key dimensions that require tighter tolerances are still defined on the face of drawing.

From there, we will transfer the casting datums to the machining datums. I would tend to take a similar approach to what I described above, positioning one hole with respect to the other hole, however you can no longer relate the outside features to the inside features because they're described on an entirely different drawing. Hence, the flat surfaces will need to be located relative to your planar casting datum and your first hole will have to be related both your machined planar datum and your v-block casting datum (with basic dimensions, of course). The second hole would then be related to the first hole (a new datum), the second machined planar datum, and your v-block casting datum.

If using a one-drawing approach (which implies a single vendor), I'd go with my previous post. If using two drawings, I'd do it like described above. At the end of the day, function comes first. Best to leave the manufacturing to the manufacturers as much as possible.