Displaying PrePlate Dimensions 1

[quest4k]

Good afternoon, I am making a drawing and it hasthe finished dimensions and preplate dimensions in parentheses. Like:
.308 (.3075)
.305 (.3045)
Then the arrow points at the part. The .305/.308 are no problem, Ijust used limit, but is there a way to get the preplate dimensions behind the finished dimensions? Thank you in advance for any and all assistance.

 

[handleman]

Allow me to be the first to say:

Make your drawing to the final dimension. It's up to whoever makes it to assure that it meets final dimensions after plating.

That being said, I don't think there's a way to do it with live dimensions other than using the limit tolerance and having one dimension above the other. If this is something you really want to do I can fiddle a macro to do it without too much effort.

 

[ctopher]

What exactly do you mean by "behind the finished dimensions"? I'm not clear.

Also, this is not standard. When I see:
.308 (.3075)
.305 (.3045)
one could assume in/mm or similar, until one looks closer.
I would suggest calling out one of the dims, a note with the proper plating spec, and note stating the dim shown is after or before plating.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[quest4k]

Thanks you for the response, handleman. It is to the final dimensions, but the machinist like it the way the old CAD system could do both and they need the preplate dimensions. The FDA also likes to see both. This just kind of confirms what I thoght about the dimensions.

 

[quest4k]

Thanks for the response, ctopher. With I say finished, I mean after plating and that it the first dimension and the the machined, preplate dimensionis the second dimension and it is in parentheses. We always work in inches so that is no problem.

 

[handleman]

So... would you want this (non-standard) dual dimensioning scheme applied to every dimension in a given drawing?

 

[handleman]

Also, is plating thickness uniform (same for every dim) or different for each?

 

[quest4k]

Thanks again, handleman. Actually it is just the dimensions were I am using the limit for the dual dimensions. These are a half dozen real critical dimensions. I was hoping to be able to keep the associativity. It is a kind of unspoken standard, extrernal critical dimension are cut -.0005. Does that make any sense?

 

[ctopher]

From my experience with the FDA, they like metric first, then inches. Calling out a plating spec, which spells out thickness, will work for them. I would call out the final dims and note that's what they are. It is up to the machinist to make the part.
SolidWorks tries to follow standards. What you are asking for would have to be done manually.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[handleman]

Ah, so internal (hole) dimensions would need to have the higher number in parenthesis. That's a bit stickier. I would venture to say there's no way to keep associativity with the pre-plate dimension out to the side.

By the way, what do you mean by "the way the old CAD system could do both"? Did the old CAD system do this automatically, or was it a hand-typed, non-associative number as well?

 

[quest4k]

Thanks again for the response. Yes teh thickness is uniform. Well, I guess I will try using text and prey there is no changes. Thanks for the help.

 

[quest4k]

Thanks again, handleman. Most holes have enough in the tolorance to not need a preplate dimension and plating usually dose not go up into holes and internal threads and the like. Plating usually stays outside on the part, unless you keep it down for a long time. Yes when the correct check box was check it was automatic and yes it kept the associativeity. I have learn not to mention that system have.

 

[ctopher]

There should be a note on the dwg stating no plating allowed in the holes. Hoping it doesn't stay down for a long time can cost $$.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[wes616]

Quest,

I often find myself in a position where I have to "dummy" something in on a drawing. When I do this, I have gotten in the habbit of marking the dummy dims, so they show up in bright blue. I am starting to put them on their own Layer, in Drawings. I also usually note this fact in (big letter)just off the drawing sheet (along with any other notes i have), so if someone else (or me in a few months - years) comes to it, they know what has been done, and the meaning of things.

Wes C.
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[wes616]

But... as has been mentioned, this could easily be handled through a flagnote...

FL XX. PLATING TO BE X.XX MAX DIM X.XX MIN DIM. DIM GIVEN ON THE DRAWING REPRESENT FINISHED DIMS. WHATEVER WHATEVER.

Wes C.
------------------------------
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[handleman]

I imagine (depending on the scale of your parts) you could kludge it to be associative. It would be quite a bit more work to set up, though. The difference between 0.385 and 0.3845 would likely not show in a printed drawing. You could:

1. Add construction geometry (a sketch point, line or whatever) to the drawing view
2. Dimension it to be the plating thickness away from the model edge your actual dimension is attached to
3. Hide that dimension
4. Add another dimension to the construction geometry that mimics the actual dimension you're wanting to show
5. Align the actual dimension with the dummy dimension with Tools->Dimensions->Align Collinear/Radial
6. Right click both the dummy dimension and the actual dimension and un-check "Center dimension"

 

[TateJ]

Are we talking about raw material dimensions vs. finished part dimensions? I'm not sure what "pre-plate" means?

For my single part drawings - I set up a second configuration (called MATERIAL). Then I input the custom properties in the MATERIAL configuration to drive the BILL OF MATERIALS. The TITLE BLOCK can then be driven from the DEFAULT CONFIGURATION.

But that might not even apply here...

Windows XP / Wireless Intellimouse Explorer
SolidWorks 2006 SP4.1 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[quest4k]

Thanks again for all of the response and ideas. Tate, this is a machined parts, that will go on to be chome plated, so several tight dimensions must be cut undersize so they will be within spec after the plater is done. Handleman, I think I will give your idea a shot, it sounds like it might work.