Dimensioning Set of Holes on From Flat to Angled Plane

[hydronicengr]

Let's say I have a thin sheetmetal part with 3 holes, labeled Hole #1, #2, and #3 in the attached picture. As shown, Hole #3 is located on an angled plane. It is important that Hole #3 is dimensioned to Hole #1. Using only linear dimensions and calling out what the angle is, how do I accomplish this?

Thanks

 

[giggity]

Do you plan on locating and orienting hole #1 to datums? Do you want hole #3 located and oriented to the datums that located and oriented hole #1 or do you want a new datum structure based off of hole #1?

 

[giggity]

Check out Fig 7-36 "Nonparallel Holes Including Those not Normal to Surface" in ASME Y14.5-2009

 

[pmarc]

You can also take a look at fig. 7-55 in Y14.5-2009.

But before anything the most important thing would be to define/establish features relative to which the hole #3 should be dimensioned and toleranced. These features are known as datum features.

 

[drawoh]

hydronicengr,

This is an excellent case for GD&T. I hope hole[ ]3 need not be accurate. Dimension hole[ ]3 from the bend. Show that your dimension is from the hypothetical sharp corner. Apply a fairly sloppy positional tolerance to hole[ ]3.

If I really need hole[ ]3 to be located accurately from hole[ ]1, I would define hole[ ]1 as a datum. I would extend the centrelines so that they intersect. I would provide basic dimensions showing the intersection point, and the angle between the lines. I would apply a positional tolerance to hole[ ]3. I would wonder how the shop would accomplish this.

--
JHG

 

[giggity]

Shop might make a fixture that would simulate the angled surfaces and then pin hole #1 if that was the datum.

 

[SeasonLee]

hydronicengr

Is this the information you are looking for? Please ref to the figure below and the attachment.( from "Dimensioning and Tloerancing Handbook" by Paul Drake Page 5-117/118 )

 

[AndrewTT]

SeasonLee, if I am reading the text and figures that you posted correctly, it seems to go against what is shown in figure 7-55 of the 2009 standard.

 

[3DDave]

Drake's second example fails because it's not an 'implied datum' problem, it's a missing dimension problem. There is no relation to any datum that is implied. The axes aren't completely located. If the axes had been extended to intersect with datum feature A and moved the dimensions to that intersection point it would work.

The standard's example shows an alternative by providing a coordinate pair that locates a point on the hole pattern axis in space and provides a basic angle between it and a referenced datum plane. It also uses the same locating dimensions to place the surface that forms datum feature D.

 

[juergenwt]

Learn how to use "Tooling Balls". Google it.

 

[drawoh]

AndrewTT,

Figure 7.55 in the ASME Y14.5 standard, however correct it is, does not conform to the OP's design intent. The surface is sloppily located from the datums. The hole pattern is yet more sloppily located from the datums, and it is internally accurate.

Drake has labelled his figure[ ]5-105 "one correct method", which it is. It provides a fixtureable datum feature to measure from. The only problems I see are that the datum depends on the fabricator not filing off the sharp edge too much, and again, that it does not meet the OP's requirements. I do not see his figure[ ]5-106 as an error. It complies with Y14.5 Figure[ ]7.55. It still does not meet the OP's requirement to be positioned from a hole on the orthogonal feature.

Given that the part is sheet metal, you cannot expect a super accurate relationship to hole[ ]3.

--
JHG

 

[pmarc]

There are different correct/acceptable methods to dimension true position of angled holes. Fig. 7-55 from the standard and fig. 5-105 from Drake's book are just two of them.

drawoh,
1. The main point here is that all the examples were given just for reference - to show that positional tolerancing is a way to go. So the fact that Fig. 7-55 does not conform to the design intent does not mean it cannot be used as a help or good starting point.
2. Fig. 5-106 is incorrect because, as 3DDave pointed out, it is lacking two horizontal basic dimensions from A to the points on the axes. If the dimensions were there, then you could say that the figure complied with fig. 7-55 from the standard.
3. And finally, I would like to understand your comment about Drake's fig. 5-105: "The only problems I see are that the datum depends on the fabricator not filing off the sharp edge too much...". What do the sharp edges have to do with chosen dimensioning scheme here? Could you clarify?

Side note:
I may be mistaken (and hopefully I am), but my feeling is that once OP read first 4-5 comments (which all encourage to use GD&T), the thread for her/him was over.

 

[drawoh]

pmark,

For figure[ ]5-105, you need careful fixture design. If you pick up the datum[ ]A face and the datum[ ]C end, everything is fine. The drawing view encourages you to fixture the angled face and the top corner at the bottom. As fabricated, you will have a radius or chamfer.

--
JHG

 

[pmarc]

The drawing view encourages you to fixture the angled face and the top corner at the bottom.

The drawing encourages me to setup the part for inspection in exactly the same way as fig. 5-106 does, because the part needs to be immobilized using datum features specified in the position FCF, and the datum features do not change between the figures.

In other words, arrangement of basic dimensions has nothing to do with how the part should be set up against datum feature simulators. Sometimes inspectors like to see basic dimensions arranged in a way that does not require doing calculations, but that is all (see link below).

http://files.engineering.com/getfil...-5630-483c-9e0e-9be3c28e0ba0&file=capture.JPG