Best Practice for dimensioning feature with draft

[SEC_MECH]

Hi,

My experience has mainly been of dimensioning metal parts with square features. Recently I am more involved with molded plastic parts with draft angles.

A square sided peg or hole would have A = B = C. But which one do we specify when a draft is applied?

I am questioning a third-party drawing who dimensioned this feature like C'. i.e. They dimensioned the theoretical intersection of the peg/hole with the neutral plane but they did so in the PLAN view. This image is exaggerated. In the real drawing the lines were so close together as to be indistinguishable from each other.

You cannot measure the dimension C or C'.

Is this the best practice?

If a molded part is just a face full of holes can ANY size dimensions be given in PLAN VIEW or would this be ambiguous. Would we require a section view for EVERY feature so that we can spell out where the measurement is taken?

Love to hear from the style gurus and standards nerds on this one 🙂

[ennujozlagam]

you wrote

If a molded part is just a face full of holes can ANY size dimensions be given in PLAN VIEW or would this be ambiguous.

my practice is indicate diameter of the circle.

Would we require a section view for EVERY feature so that we can spell out where the measurement is taken?

yes for better understanding for fabrications.

[TESTPC]

Late to the party, but perhaps someone who finds this in search will benefit.

Consider applying the ASME Y14.8 standard to your application. It's for castings, forgings and molded parts.

Section 5.7 of the most recent draft standard says dimensions shall be considered to be at the mold line unless otherwise specified. This is the theoretical or virtual line generated at the intersection of the extended draft and the dimensioned end of the feature. That is what occurs in your C & C' dimensions. (I'm guessing that C' is just an unconventional way to indicate a reference version of C).

IMO it should be shown in section for clarity, especially since the root fillet is so large. In the section view you can dimension wherever is best for your application, since it is clear what you are specifying. You can show the dimensions as reference in plan view if you want them there for some reason.

When dimensioning only in plan view, there are a few optional approaches that are subtly different.

1. Have a general note that says "UOS DRAFT ADDS MATERIAL". Then dimension in plan view such that draft always adds material to the part. So for a screw boss you would dimension both the OD and the ID at the tip of the boss. If these are filleted, make the dimensions to the theoretical mold line.
2. Explicitly use the +DFT modifier on your dimensions. This indicates that the listed dimension applies at the smallest point, and the draft causes the numerical value to increase from there. So for a screw boss, you would dimension the ID at the root of the hole, the OD at the tip of the boss, and mark both as +DFT.
3. The previous two can be inverted as either "DRAFT REMOVES MATERIAL" or -DFT.

AVOID using the shorthand +DRAFT. Some people use this in place of "DRAFT ADDS MATERIAL" while others use it as a long-hand for the standard-defined +DFT. Stick with the standard or clearly document what your notes mean.

These are specifications for draft are optional because that standard wants to make it possible for your drawing to be "at the molders discretion" if the part designer is unsure of the parting line. Leaving the draft direction vague can be a pro in some applications. But for a screw boss, we all know which way the draft needs to go in 99.999% of the cases. (With the rare exception being when negative draft is needed to keep the part on a particular mold half when the mold opens.)