Hi everyone I am little bit confused about dimensioning the equidistant holes in the drawing. I am attaching the jpeg file please have a look. if I don't want to dimension the linear distance of all the holes how should I mention that.
E.g. add a Total distance where it would read 150 and edit it with "3x50=150"
Add "TYP" to the pitch dimension.
"TYP" is an abbreviated form of "Typical", and is often used to signify that several dimensions are identical to the one shown.
You must, however, be careful in its use, because it is easy to introduce ambiguity. If the part has 2 sets of holes on a 50 pitch, for example, one pitch should always be shown on each set.
This is one way I do it. Obviously I wouldn't show the dimensions at the bottom, these are just so you can see what the dim's at the top represent.
I also sometimes use TYP, as John has mentioned, and probably would if all the holes had the same cross centre pitch.
I used to work at a place where they liked the "aXb=c" format, but I weaned them off it, because it is much harder to make that style parametric than it is the "n HOLES dia a THRO" with a pitch dimension and a TYP approach.
The only way I could figure out how to make the "aXb=c" format parametric was to make a special parameter which was equal to n-1, where n was the number of holes, then use that in an equation in a note, etc. etc. ...
You see what I mean. It's a perfectly valid way to dimension the features, but it makes a lot of work, due to the limitations of 3D CAD software, to keep it all parametric.
Of course, this was back when I was using Pro/E - in SW it may be trivial...
I have found that in order to have the AxB=C note work you can create a dimension for the first dimension and one for the overall distance. Then I create the note picking the dimensions in the appropriate turns so they are placed where needed. After placing the note I hide the original dimensions. I use this method for slots and the like.Thinking about this now this method will not give the witness lines you want for dimensions though. Not sure how to get that to work, and I just attempted to place a dimension into the note of another dimension but that didn't work.
Everywhere I have been we just place the first dimension and use "typ".
From ASME Y14.5
ASME? I don't know about that - all metric over here!
BS8888 doesn't show it (I think) - although I'm not sure there is anyone alive who has looked at every page of every cross-referenced standard in that particular document!
It does raise the question, though:
If that is the way ASME recommends it be done, why is it not easy to achieve in Pro/E and/or SW? I'm sure they were both designed with the US market in mind, with us Europeans at best an afterthought.
ASME includes metric. SolidWorks seems pretty well tuned to follow ASME standards, at least for what I've been doing. (Except for center marks and center lines.)
Thanks a lot everyone....
I've attached a solution to your OP, but I'd recommend simply "3X 50".
I wouldn't do any math because, as stated previously, it's not dynamic.
But neither is my recommendation. Nothing is.
So keep this in mind so that you minimize your exposure to potential errors from future changes.
Also, if you do opt to do the math, it's a reference value and it (the sum) will need to be placed in parentheses.
Just curious, will the accumulative stack affect the mating part?
If you do want/need dynamic, you can combine linear patterns, global variables and custom properties to achieve your OP, see attached.
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