How to define a feature that isn't in the nominal profile

[flash3780]

I ran into an interesting scenario that I wasn't sure of the best way to handle. I'd like to define a feature that exists at MMC, but doesn't exist in the nominal profile of the part.

The particular geometry that I'm looking at is a machined radius that breaks out of a cast surface. I'd like the surface to continue on at an angled taper when the casting is at MMC, rather than for the radius to continue to turn outward. Trouble is, I'm not sure how to define the taper, since it doesn't exist at nominal tolerance.

I suppose that I could model the casting at MMC with a unidirectional profile, but I can see that causing all sorts of trouble with the casting vendor. Is it legal to define the remainder of the profile with phantom lines? Thoughts?

Thanks for the help.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com

 

[MechNorth]

Phantom lines are fine, but you should add a note indicating what they represent.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[CheckerHater]

First, I would blow-up the undercut area so details are seen clearly.
Then, use phantom lines.
Then pick the appropriate note. The features / dimensions that disappear after machining sometimes are marked as “NON-MANDATORY REQUIREMENT”. Another good term is “PEMISSIBLE”. It implies that feature may appear under some conditions.
Just a personal approach though.

 

[flash3780]

Thanks for the advice. I put together a sketch of the definition, but it seems to be a bit of a mess. Any suggestions for cleaning it up?

PNG Image
SVG Image

 

[flash3780]

I forgot to include it in my sketch, but the vertical surface is located with a +/- tolerance. I believe that's legit per ASME Y14.5-1994 (kind of a combination of figs 6-18 and 6-23)... but check me on that.

PNG Image (Updated)
SVG Image (Updated)

 

[flash3780]

Whoops, that second SVG Image should have been this one.

 

[MechNorth]

Looks ok, except the +/- tolerance. The figures that you cite both reference directly opposed points, which makes them features of size. What you indicate seems to be a stepped surface, not a feature of size, so +/- is not the preferred means of locating that surface. Profile of a Surface is more appropriate.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[flash3780]

Jim,
Thanks for the insight. So, you're thinking profile along the whole surface, then? Works for me, but I'll have to sell it to the product definition folks (seems like profile tolerance scares them for some reason... some bollocks about difficult inspection).

Well, it seems like a bit of a mess, but I can't think of any cleaner way to present it. They're currently specifying a maximum step from the cast surface and that undercuts are not allowed in a note. That's fine, but it'd force the manufacturer to set their cutter path based on wherever the cast surface winds up for each individual part.

I'm suggesting that they move the nominal radius north a smidge and forget about the max step requirement, but set the tolerances such that you never have an undercut. Should be a cost savings there, I think.

Anyhow, here's the updated doodle:
PNG Image (Updated)
SVG Image (Updated)

 

[MechNorth]

That looks about right. Personally, I'd force a cut deeper into the radius to ensure it's cleaned up regardless; "olde days" wouldn't have been an issue because manual machining would have contacted the surface before starting the cut but CNC likes to start at a predetermined location (unless they have force feedback capability in the mill/lathe).

I just love when people say Profile is too hard to inspect ... I quickly provide a redirection in their geometric philosophies.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[flash3780]

Jim,
I had them set the radial position such that when the cast surface is at MMC and the machined surface is at LMC the surfaces line up exactly (i.e. no step); the intent is to avoid an undercut since it would unnecessarily weaken the part. I also amended the note to read:
[tt]TAPER MAY NOT BE INCLUDED IN MACHINED PROFILE DEPENDING ON MATERIAL CONDITION. BLEND BREAKOUT TO R1.3 [R.051] MINIMUM.[/tt]
I think that the blend note should sufficiently clean up the cusp.
Thanks for the advice... I had a hard time finding an example of this sort of breakout, but I think that the definition above should adequately communicate the requirement to the manufacturer.
Defining geometry that doesn't exist in the cast profile is a bit tricky; I wasn't sure if using phantom lines was legal, but I think that the note clears things up in this instance.

 

[MechNorth]

Sounds good.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com