I just need a double check on following tolerance stack calculation. What would be the minimum and maximum distance between bottom surface of the part (datum feature C) and hole surface using worst-case approach?

Forget about first sketch - no basic dimensions for hole were given there.

• http://files.engineering.com/getfile.aspx?folder=a4d20139-cd51-4715-9599-a4

This may help:
http://www.engineersedge.com/true_position.htm

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

For us to 'double check' shouldnt' you tell us what you think it is?

I'm thinking...

X=30-1/2 max hole dia-1/2 pos tol dia - 1/2 MMC bonus tol.

However,  in practice since B & C don't have physical datum identifiers it will be tricky to say which is 'X' and which is the other side of the hole on a real part.

KENAT,

Let's say there is a groove thru the upper surface of the part, so there is clear indentification which surfaces are datum features.

I am asking because I want to check if datum features perpendicularity controls should be somehow involved in this calculation. In my opinion yes, so I would add to the formula you gave perpendicularity factor.

I suppose it depends on your definition of 'X'.

If it is the distance from simulated datum C then I think what I put is right.

If it is the distance from 'lowest point' of datum surface C then I suppose yes, you should also subtract the perp.

pmarc,

   The smallest distance X occurs when you have the largest hole at lowest allowable position.  I am assuming that X is located from Datum_C.  This is not necessarily the same thing as the distance from the actual edge.

   Note that with the hole at Ø15.2mm, your positional tolerance is Ø0.3mm.

   X_min = 30mm - 15.2mm/2 - 0.3mm/2 = 22.25mm.  

   Datum_C is the portion of your bottom edge that touches your fixture.  This means that the maximum perpendularity error will be towards your hole.  This could bring your separation down another 0.1mm.  

               JHG

Kenat,
I was rather thinking of distance between part features not the hole and simulated datum feature C.

For your information my original calculation was:
MAX = 22.55
MIN = 22.15

The max is 22.55.   The min is 22.25
 But that's assuming you are asking for the distance from "datum C" to the hole's rim.  If you are asking for the distance from "datum feature C" to the hole's rim, then the min would be 22.15 because of the perpendicularity's effect on the form of the bottom surface.

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

Belanger

There is no doubt about the perpendicularity's effect on the form, will this also effect on the max 22.55 and result at 22.65 ( 22.55 + 0.1 ). Please let me know if I am wrong.

SeasonLee
 

SeasonLee,

I agree with Belanger because of rule #1.... Perfect form at MMC

max value: 22.55
 

It's still 22.55, because the position of the hole is from datum C, and datum C is always formed by the high points along the bottom surface.  So there's no additional maximum due to form; only the minimum is affected by form.

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

Thanks Belanger,what you said is exactly right.

SeasonLee

Sure, SL.   Stacks are always fun, aren't they?  :)

 

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

Hello i am a bit new to this mechanical stuff and i am trying to understand how you worked this out?

Would sombody break it down for me so that i can understand each part.
drawoh, How did you get the positional tolerance Ø0.3mm from the hole at Ø15.2mm.
If you could explain i would be very gratefull.

Thank you.

The smallest distance X occurs when you have the largest hole at lowest allowable position.  I am assuming that X is located from Datum_C.  This is not necessarily the same thing as the distance from the actual edge.

   Note that with the hole at Ø15.2mm, your positional tolerance is Ø0.3mm.

   Xmin = 30mm - 15.2mm/2 - 0.3mm/2 = 22.25mm.  

   Datum_C is the portion of your bottom edge that touches your fixture.  This means that the maximum perpendularity error will be towards your hole.  This could bring your separation down another 0.1mm.    

The attached drawing makes sense to me.  

Peter Truitt
Minnesota

• http://files.engineering.com/getfile.aspx?folder=6d9f467e-f34d-4659-8e07-4f

Attached is the drawing I'm working with, I'm trying to find the Max and Min for Dim (X)
My Drawing could somebody explain step by step the procedure I need to go through to find the Min and Max, like I said im a new to this game so explanation for dummies please.

Thanks all very much appreciated.

• http://files.engineering.com/getfile.aspx?folder=b8488046-406b-49aa-9d54-ae

Max = 4.25 and min = 3.75,   because 4 ± 0.25 is the spec for dimension X given on the print!

(FYI, the 15.15 should not be basic.)

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

bluehonda,
J-P is right. There is nothing to calculate except of taking min and max values of 4+/-0.25 dimension.

what would be a better way to dimension this part up then? what do you suggest the 15.15 should be if not a basic dimension.
I am trying to maintain the hole position in relation to the edge of the plate.
Also doesnt the geometrical tolerance (Hole position Ø 0.25)have any impact on dimension (X)?
Would it be better to dimension the edge of the plate to the arc of the hole?

To have the geometric tolerance control the location of the holes from the edges, you need to have datum letters (representing the edges) be mentioned at the end of the GD&T box.  I'd recommend the back face of the plate as a datum too ... call that datum A.  Then have the bottom edge labeled as datum B, and the left edge as datum C. Then have A, B, and C given after the 0.25 section of the GD&T callout.   The 15.15 would stay basic, but now your 4 mm dimension would also be basic (and drop the ±0.25).  

Consult any simple GD&T reference book/guide for an example of this scenario.

Your answer for "X" would then be a max of 4.125 and a min of 3.875, because the given geometric tolerance is diametrical (think of the tolerance zone as being centered exactly at 4.00 so it translates to .125 in any radial direction).  The max distance between the holes would be 39.25 and the min would be 38.75.

 

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

First of all I would suggest not to use coordinate dimensioning (4±0.25) for locating left hole from the left edge of the part. I would recommend changing it to basic dimension, assigning three mutually perpendicular surfaces as datum features A, B, C (like in my original example) and put position tolerance to the pattern of two holes with the reference to A, B, C. This would at least eliminate ambiguity of current dimensioning scheme.

I do not think you want to dimension arc of the hole from the edge of the plate. In most of similar cases position tolerance is applied to control location of holes axes relative to other features.

Why the hole position (Ø 0.25) has no impact on dimension (X)? Because you directly defined that the distance between axis of left hole and left surface of the part is 4±0.25. With your dimensioning scheme position tolerance is important only when any relationship between both holes is considered.

Quote (BLUEHONDA):

...
drawoh, How did you get the positional tolerance Ø0.3mm from the hole at Ø15.2mm.
If you could explain i would be very gratefull.

    The hole has a positional tolerance of 0.1mm diameter at maximum material condition.  It applies at the minimum diameter of 15.0mm.  As you increase the actual diameter, you increase the positional tolerance.  At 15.2mm diameter, the positional tolerance is 0.3mm.

               JHG

Could anybody show me how i would work out what the smallest amount of material would be left between the hole and the outside edge of the pad.
Several people have had a go at this and given me different answers.
Is there a quick and easy method of working this out? And please bare in mind that I'm very new to this stuff, so explanation for dummies please.

Thank you all.
 

BLUEHONDA,

Look to attached presentation. It is showing an example of how you could have thought about the stack I asked for a double check at the very beginning of the post. I tried to explain it as simply as I could. Hope this helps.
http://files.engineering.com/getfile.aspx?folder=e315da8e-d4a2-4bae-9e71-85710eb4d765&file=Tolerance_stack.pdf

P.S.: If you are asking for a quick and easy method of dealing with tolerance stacks, I would say it really depends on one's experience, preferences and how complicated a stack is. The method I like to use (it is not the one I showed in the attachment) is really easy and consistent for me, but that does not mean it would be clear for you. First of all try to do as many stacks as possible, choose different calculation methods as described in different GD&T books (e.g. Krulikowski, Fisher or other authors) and you will quickly notice which one is most suitable for you. Additional Tolerance Stack-up training would also help for sure as you you seem to be at a beginner level.  

Excellent step by step explanation, pmarc.

SeasonLee

pmarc
Am I correct understood from your PostScriptum that stackup results can be differ and it's depend from calculation methods (e.g. Krulikowski, Fisher or other authors)?

No, the answers should be the same.  He's saying that you may prefer one method over another.

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