How can I convert these linear dimensions to GD&T?

[ejsam]

How do I convert these linear dimensions to GD&T? Can I use angularity with a cylindrical tolerance to define the angled feature? The theoretical intersection point is a critical dimension

 

[Burunduk]

Which dimension to the theoretical intersection is critical? Is it 150.85±0.05 (which BTW looks difficult for that length) or 9.75±0.05? Or both?

 

[3DDave]

What mates with the theoretical intersection point?

What mates with the features of this part?

Would you be willing to use datum feature symbols and feature control frames instead of the marketing term "GD&T" ?

We might agree that "theoretical" isn't correctly spelled the way it is on that screen shot, but some may not.

Then we can kick around what requirement "BLEND SMOOTH" defines.

 

[ejsam]

Sorry this is what I could send trying to markup on a phone. There's a nut that gets screwed on the back side of the part and there's a hex bit that sits on the front side. The theoretical point is the center of the ball hex. The back face controls the distance of the theoretical point and the 9.75 distance - 2mm where hex sits in the angled housing is critical.

 

[3DDave]

It looks like using a position tolerance on the bore the bit sits in and a profile tolerance on the face that locates the bit in the bore with the inside diameter of the main body as the primary datum feature for each feature control frame will perform the function. Since the contact with that main body is just two small areas those would be best dealt with as datum feature targets and a profile of surface tolerance of those surfaces to those same datum feature targets used as a control for mutual orientation.

The tolerances should be set by a dynamic FEA analysis to determine the limits relative to the contact force on that coupling between the ball hex and the hex recess.

It looks like a dental tool. I think those usually use crown gears to avoid the need for the small acceptable tolerances this is likely to require to avoid beating the coupling so badly.

 

[ejsam]

Hi Dave

Thank you for your input.

Can you check the attached image and give your feedback. I know datums need to be mutually perpendicular but Solidworks does allow me to use the angled bore as a datum C without giving me any errors. Do you think its something I could do use the angled hole as datum C?

 

[3DDave]

Datum features do not need to be mutually perpendicular. Ask Solidworks users why it acts that way.

 

[Burunduk]

ejsam,
Here are some general thoughts:

First, as 3DDave indicated, datum features aren't required to be mutually perpendicular. The datums derived from the datum feature simulators of the datum features, are used to connect the part to a datum reference frame that is constructed from 3 mutually perpendicular planes.

In your last drawing, the face that is at the basic distance of 9.75 from the intersection point is not controlled for location relative to your chosen datum reference frame, because there is no profile tolerance applied to it. I would also say the functional face must be not this one but the internal one, where the shoulder of the bit sits. So I'm not sure why in the original drawing with the directly toleranced distances, 9.75 was tightly toleranced, and why you indicated that it is critical.

In addition, for a long part like this, it may be useful to consider two datum reference frames, one at the interface with the rear nut, and the other at the front where the hex bit sits, to control features that have a functional relationship with the bit. The primary and secondary datum features used to derive the front datum reference frame could be the ⌀4.02 opening and the face that contacts the shoulder of the bit, and they should both have a controlled location and orientation relationship relative to the rear datum reference frame.

Also, if you need precise location and orientation of features, you may want to reconsider the datum shift resulting from datum feature A referenced at MMB and the bonus tolerance resulting from the tolerances specified at MMC. These are suitable where you mainly care about parts fitting together, and less concerned with precision.

Just out of curiosity, how does that part gets inspected?

 

[ejsam]

Thank you Dave and Burunduk for your valuable feedback.

Tbh, I'm not sure how the manufacturer is going to inspect it.

The last drawing was a mistake and we are trying to correct it where the critical 9.75 is given from the outside face when it needs to be from the face where the bit shoulder rests. I did add a profile tolerance on the face where the bit sits.

Solidworks MBD did allow me to use the angled 30 degree hole as datum C so here is screenshot of it looks like.
I made the main body ID 6.25 as my Datum A , Angled Bore Dia 6.25 where the Bit sits as Datum B and the back face where the nut fits as Datum C. I am sending a picture (highlighted in blue - functional faces).

Please let me know if I am heading in the right direction

 

[ejsam]

Here is a picture of the Datums

 

[ejsam]

I was thinking if I could use two single segments like here if I want to keep the Main body ID 6.25 and the 13 mm in relation as datum A-B and the angled Bore ID as datum C.

 

[Burunduk]

ejsam,
Your datum feature selection for a given set of datum references in a feature control frame should either reflect the assembly interaction between the considered part and the part that constrains it in assembly, or the interaction between the part and the part constrained by it.
The A@M, B, C@M datum references specified in several feature control frames is a combination of both, and therefore neither of them. Its functional value is questionable.