Quantcast

Print reading question

Help Support HMEM:

goldstar31

Well-Known Member
Joined
Feb 20, 2010
Messages
2,786
Reaction score
864
Location
Twixt Tyne and Tees
But gentlemen MOST if not all of the erudite conversation is from full size operations and NOT from what most of us have in our own badly funded home workshops where either a badly in need of replacing our repair of an ancient lathe or mill or perhaps some badly equipped Chinese little misery is the norm.

The place seems dotted with repeated and repeated questions- and sometimes doubtful answers about the actual problems which beset most of us.

Here it suggests some impossible dream removed from ever becoming reality- at least for me.

Perhaps someone else might dare to agree with me?

I should perhaps explain that there is a precedent in the past where I recall contributors talking about thousands of an inch and only possessing rulers and lathes without dials and TPI which would only produce 62.5 gradations per revolution.

I feel sorry for those who are trying hard in solving the problems of their own little world of making models and things to go with them.
 

Misterg

Member
Joined
Apr 20, 2020
Messages
11
Reaction score
3
Location
UK
I thimk that CADs should be modified so that the drafter can place non-required dims into the drawing, maybe in greyed colors/lines so one cannot mistake it for a requirement.
I doubt that anything needs modifying - this is the exact purpose of "Reference Dimensions" - they appear in brackets on prints (or with the suffix 'REF' depending on drawing standards). I can't speak for all CAD programs, but both Creo and Fusion360 allow them.
 

goldstar31

Well-Known Member
Joined
Feb 20, 2010
Messages
2,786
Reaction score
864
Location
Twixt Tyne and Tees
Well Igot one response from an a young-ish correspondent who cou;d do with a bit of my experience on a somewhat ancient- well younger than me- lathe.

Thanks Jon being told in real terms that there IS a real world out there.

Oddly, I've just received a fancy DRO to fit on my Myford. Laughingly, it would look quite amusing on a 7 by ? Chinese latheo_O
 

nealeb

Member
Joined
Jun 24, 2014
Messages
14
Reaction score
6
As an amateur (mechanical) engineer and enthusiastic 3D CAD (F360) user, I have been finding this debate interesting, amusing, and occasionally instructive by turns!

I have given a number of 3D CAD tutorial sessions to fellow club members, and I have to say that it is a lot easier to teach people with no knowledge of CAD than those with many years of experience of 2D draughting. The reason is partly tied into some of points of view expressed here.

I bang on to my "pupils" the need for a3D model to express "design intent" and not embody good 2D engineering drawing practice. In the case of the countersink, what is going through the designer's mind is, "what is the minimum depth of the countersink so that allowing for bolt manufacturing tolerance, the head will be at least, say, 10thou below the surface." In my hypothetical 3D model, this is what I would construct. Everything else follows on from that. Now, some time downstream, the designer has to produce engineering drawings to go to the workshop. I know that in F360, these can have as many dimensions as you wish, whether the drawing is over-dimensioned or not. These dimensions (to whatever number of decimal places you as designer choose) will never disagree because they all derive from the original 3D model (and if that model is updated, the dimensions will automatically be recalculated). The question is, though, to what extent the designer should define or assume the details of the manufacturing process and thereby choose what dimensions to put on the drawing? Should he know what the point of the countersink is? Sharp, 20thou, 40thou, flat? How will the machinist set his machine? Will he end up with a machinist banging on his desk and saying that he doesn't want to be told how to do the job? So, he might just translate the initial design intent into external diameter of the countersink and let the machining experts work out how to achieve that. With a simple bit of trig, perhaps? Maybe there is a production engineering stage between designer and machinist who makes these decisions, and might even ask for specific relevant dimensions on the drawings to suit the local ways of working.

As for inspection - design intent could be checked with a simple gauge that looks like a dummy bolt made to max tolerance conditions of the bolts to be used. Does it sit 10thou below the surface? Do the drawing dimensions required by the inspection department have anything to do with the dimensions needed to manufacture the piece? Quite possibly not. Should just one drawing have all the dimensions required by both parties, even though they might over-complicate and confuse things? Should there be two drawings derived from the same model (ensuring consistency) aimed at the specific user?

I know from my own experience that as designer and machinist, what I put in the model for design purposes is not what I want for the machining process. Great thing about 3D CAD is that it separates the two, while guaranteeing consistency (although I look forward to the F360 version that will update my scruffy and oil-stained drawing prints hanging over the lathe as soon as I update the computer 3D model!)
 

cds4byu

Active Member
Joined
Apr 28, 2014
Messages
43
Reaction score
9
ISO has a specification for the dimensions and the dimensioning practice for countersunk screws. ISO 15065.

The CAD systems I work with automatically create both the numerical dimensions and the dimensioning practice in conformance with the standards.

Carl
 

Richard Carlstedt

Well-Known Member
Joined
Jul 9, 2007
Messages
71
Reaction score
30
Location
Green Bay ,Wisconsin
Nealeb, your quote in post 64
" Maybe there is a production engineering stage between designer and machinist who makes these decisions, and might even ask for specific relevant dimensions on the drawings to suit the local ways of working "
is spot on !

I am a retired Manufacturing Engineer
Not all companies use this resource for making a product. Several firms I worked for believed in Mfg Eng.
At one Die Maker Company I worked for, they were pulling their hair out due to errors and hired me. After a year there, I showed the owners that 82 % of the drawings/specifications had errors. So in essence I had to "redline" all those CAD drawings so the machinists could make the parts that would fit other parts. I am proficient in Solidworks and know that many "adaptations" can be made to prints, but designers either have no knowledge of manufacturing steps, do not know their CAD system, will not accept changes , resort to standard protocol like ISO or whatever , and therefore make it difficult to manufacture . Now stop ! There is one area that is near impossible to get corrected....a "Customers" drawing... When you have those, all bets are off . But for your own shop or company, there is no reason a "note" cannot be provided spelling out the objective of a dimension. Last note, ALL CAD users are taught to never duplicate dimensions...Why ? That rule is dumb. First, that "concept" is a holdover from Manual drawings because it could produce errors. In a CAD system (3D) where a model has been created. It is impossible to have two different dimensions for the same measurement. . It can save minutes/hours on a print with many dimensions so the machinist does not have to search for it.
This discussion is a huge subject so I will stop here
Rich
 

willray

Well-Known Member
Joined
Dec 10, 2014
Messages
57
Reaction score
8
Will:, I keep laughing at that number: .0627--That number would not even be used in rocket science, as far as I know. there is no reason to use four places for a screw in amateur usage! for us Amateurs, .06 (1/16th") is just fine. the difference is less than the thickness of paper and about the thickness of fine hair. I say "fine" hair for a reason: not all hair is the same thickness! 1/16th is .0625. so the diff between .0627 and .0625 (1/16th) is two ten-thousandths! Add up the weight on that difference for 100,000 holes, say in a Boeing jet, and it won't change any parameters or be enough to make the plane crash or disintegrate. It won't weigh any significant amount.
Richard, I was just quoting the figure being discussed in a previous post. However, I would suggest, if you're going to make "eh, close enough" approximations for an alternative dimensioning strategy to the "82 deg at .225 diameter" specification, that it would be wiser to choose .063 depth of the countersink as the simplification. 1/16 is a nice fraction, but since few of our machines speak to us in fractions, it's not really much friendlier at the handwheels than .0627. Given the limits of our typical dials, we're stuck with .062 or .063, and since we don't know how much wiggle-room the original designer left us in the .225 dia. spec to prevent the screw head from being proud of the surface, shorting the depth by aiming at .062 (or less) in a redimension seems unwise.
 

willray

Well-Known Member
Joined
Dec 10, 2014
Messages
57
Reaction score
8
In a CAD system (3D) where a model has been created. It is impossible to have two different dimensions for the same measurement.
Sadly, no, it is not impossible - or at least not impossible for a feature to have two different dimensions "in the drawing" depending on which dimensions you add/follow to arrive at the feature's specification. And this is why it remains important to not over-dimension parts.

If you would like an example, simply draft yourself up a right triangle with both legs of length 1 in your CAD program and dimension both legs and the hypotenuse, as well as the angles. Unless your CAD program represents the length of the hypotenuse as sqrt(2), you now have a drawing where /some/ dimension on the drawing, must be false. If you provide that drawing as a specification, the end-user must make assumptions regarding which dimension(s) are to be ignored.

With a right triangle, one might believe that any reasonable machinist would assume that the right angle, and legs are the defining dimensions, and that the hypotenuse and 45-degree angles should simply be allowed to fall where they will. With drawings that are more complex however, over dimensioning rapidly makes it impossible to figure out which dimensions are actually the intended specification.
 
Last edited:

nealeb

Member
Joined
Jun 24, 2014
Messages
14
Reaction score
6
And that is why, particularly when using 3D CAD, you have to differentiate between "design intent" as built into the model, and the engineering drawings that are produced from it. In the days of manual 2D draughting, this difference didn't really exist as there was only ever going to be the one drawing, with its views and sections and so on (and a lot of mental effort by the draughtsman/designer to ensure that these were all consistent). In the example from the previous post, my model would be fully defined by two sides and the right-angle between them. In F360, if I tried to put a dimension (at the model-building stage) on the hypotenuse it would quite rightly tell me that it was over-specifying. In fact, it would add the calculated dimension but put it in parentheses as a flag. However, when I come to produce engineering drawings from the same model I can select any combination of sides and angles to dimension because these are derived from the model. I would choose whichever best suited the downstream process - in my case, what I needed to make the part in my workshop!
 

willray

Well-Known Member
Joined
Dec 10, 2014
Messages
57
Reaction score
8
However, when I come to produce engineering drawings from the same model I can select any combination of sides and angles to dimension because these are derived from the model. I would choose whichever best suited the downstream process - in my case, what I needed to make the part in my workshop!
Actually, it can be a bit worse than that. You need to understand and choose appropriately so that you don't lose the design intent, when making choices about which dimensions to carry through to your production process. With the right-triangle example, if you choose to carry the hypotenuse and the two 45 degree corners down to your (let's call them) "shop drawings", and you faithfully produce parts to that drawing, your triangles will _not_ have 1-inch long sides, and you will have failed to produce parts that meet the design intent.

This is a bit of a contrived example (though completely real, and it's terribly easy to land in this situation in a less-contrived drawings as soon as you have anything other than parallel or perpendicular features), but, given this drawing, a) how long is the block, b) what is the angle the sloped section makes with the horizontal, and c) if you, and two other machinists independently choose subsets of those dimensions to carry down to your "shop drawings", how likely is it, do you think, that you will all produce parts that are identical?

Screen Shot 2020-08-10 at 9.32.39 AM.png


(This doesn't even /have/ derived dimensions - all of those are true dimensions, to the precision at which I'm working. And yet, even without derived dimensions it's still confusing as !#@$, because it was dimensioned by a lazy person who didn't think about conveying the design intent. Derived dimensions that are not clearly understood as derived, _or_ not clearly understood as to _how_ they were derived, make hash of understanding the design intent even more quickly. This is part of the reason why it's often important to leave the job of deriving the dimensions to the machinist, or process-design engineer - then they understand _how_ the derived dimensions were arrived at).

Overdimensioning is a curse. I quite like _derived_ dimensions (when they are represented as derived), but overdimensioning, when it's not obvious which are the derived dimensions, ablates the downstream user's ability to understand the design intent. "Shop drawings" that omit design dimensions in favor of "more relevant to the machining process" derived dimensions, make it impossible to determine whether the thing you're making, meets the design specifications. "Instructions", as proposed by William Mays, when they are produced with a knowledge of the design specifications, are wonderful, but they can rarely be used to check compliance with the design spec.

I really don't want to call the hue and cry for "gimme all the dimensions" a product of laziness, but a good designer or draftsman puts considerable effort into choosing the appropriate dimensions to represent, so that the design intent is properly conveyed. Studying those choices, and arriving at an understanding of the design intent, is part of what should be the machinist's job, and should be part of the treasured skill set that sets the machinist apart from the ape.

I would never argue that that job should be made harder by the provision of badly-dimensioned drawings, and lord knows CAD programs produce some awfully lazy "draftspersons" and badly-dimensioned drawings. However, this job or hobby should not be "Oooh - Numbers! Grugg turn dials now!".
 
Last edited:

Richard Hed

Well-Known Member
Joined
Nov 23, 2018
Messages
445
Reaction score
107
Location
Seattle
Richard, I was just quoting the figure being discussed in a previous post. However, I would suggest, if you're going to make "eh, close enough" approximations for an alternative dimensioning strategy to the "82 deg at .225 diameter" specification, that it would be wiser to choose .063 depth of the countersink as the simplification. 1/16 is a nice fraction, but since few of our machines speak to us in fractions, it's not really much friendlier at the handwheels than .0627. Given the limits of our typical dials, we're stuck with .062 or .063, and since we don't know how much wiggle-room the original designer left us in the .225 dia. spec to prevent the screw head from being proud of the surface, shorting the depth by aiming at .062 (or less) in a redimension seems unwise.
Of course.
 

Richard Hed

Well-Known Member
Joined
Nov 23, 2018
Messages
445
Reaction score
107
Location
Seattle
Sadly, no, it is not impossible - or at least not impossible for a feature to have two different dimensions "in the drawing" depending on which dimensions you add/follow to arrive at the feature's specification. And this is why it remains important to not over-dimension parts.

If you would like an example, simply draft yourself up a right triangle with both legs of length 1 in your CAD program and dimension both legs and the hypotenuse, as well as the angles. Unless your CAD program represents the length of the hypotenuse as sqrt(2), you now have a drawing where /some/ dimension on the drawing, must be false. If you provide that drawing as a specification, the end-user must make assumptions regarding which dimension(s) are to be ignored.

With a right triangle, one might believe that any reasonable machinist would assume that the right angle, and legs are the defining dimensions, and that the hypotenuse and 45-degree angles should simply be allowed to fall where they will. With drawings that are more complex however, over dimensioning rapidly makes it impossible to figure out which dimensions are actually the intended specification.
Yes, you are correct. I was not clear on what I meant. What I am thimking is that, say you have a part 4 units long but it is broken up into 3 or 4 sections like two bearings on the ends, a larger section then a larger yet section. As a machinist I might need to pencil in two dims that I wish to know over and above the printed dims. like from the left end to the end of the third section which has already been dimmed properly but sometimes it is necessary for other dims than the proper ones. and as for myself, I would prefer to have a toggle system in my CADs to turn on or off such a capability. For other peeps, of course, like work drawings for sale or whatever, you wouldn't do such a thing. It's only for my own convenience that I don't have to use a calculator to pencil them in--let the CAD do the work. Most of all, I really do not like machines (or even people) telling me how to make something or what to do or not to do. I take instruction and advice nicely but NOT orders.
 

willray

Well-Known Member
Joined
Dec 10, 2014
Messages
57
Reaction score
8
Yes, you are correct. I was not clear on what I meant. What I am thimking is that, say you have a part 4 units long but it is broken up into 3 or 4 sections like two bearings on the ends, a larger section then a larger yet section. As a machinist I might need to pencil in two dims that I wish to know over and above the printed dims...
Hi Richard. Mostly, I was railing against the suggestion that "Don't overdimension a drawing is a useless holdover from the days of manual drafting", and that since "computers don't make drafting errors", this convention was now irrelevant. I'm sure you are already familiar with the issues, but there are so many self-taught/only-ever-driven CAD jockeys that think that this is true, that I believe this bears being explicit about.

While computers can be reasonably argued to make far fewer simple math errors than human draftspersons, the prohibition against overdimensioning was only ever peripherally about _mistakes_.

It was (and is) much more about preventing the possibility of a feature being able to be interpreted as located at more than one location, or having more than one dimension, with the difference depending on the path one takes through the provided dimensions. Even without mistakes, this can easily happen due to "invisible digits" that can creep into dimensions, most obviously as a result of trig relationships defining the position of features. The good designer or draftsperson makes sure that only those dimensions that allow the machinist to correctly position or dimension the part, are represented on the specification drawing.

Now, the wonder of the enabling technology of the computer doing the math for me to calculate derived dimensions to help me work through my machining strategy without needing to spend hours with a calculator, or a designer providing process hints like William May's "plunge your countersink .063 inches", those kinds of benefits I'll take any day of the week. I just wish more of today's designers and CAD jockeys understood that just because "the computer doesn't make math errors", doesn't suddenly make overdimensioning ok, or reduce the amount of thought that the designer needs to put into choosing how to dimension the features to correctly communicate the design intent!
 
Last edited:

IanN

Well-Known Member
Joined
Aug 16, 2007
Messages
130
Reaction score
48
Location
Bath, UK
The OP's image clearly describes the countersink requirements according to drafting standards. I don't know what the fuss is all about.

Eugne
Hi Eugne,

I think you are missing the point - the criticism of the drawing is not whether it is correctly drawn, but is from people complaining that international drawing standards are wrong and that their personal way of doing things is right

Having worked in engineering for over 40 years I have come to hold such standards with great respect (I have seen the time, effort, consultation, consideration and debate that goes in to the process of defining them)
 

IanN

Well-Known Member
Joined
Aug 16, 2007
Messages
130
Reaction score
48
Location
Bath, UK
But gentlemen MOST if not all of the erudite conversation is from full size operations and NOT from what most of us have in our own badly funded home workshops where either a badly in need of replacing our repair of an ancient lathe or mill or perhaps some badly equipped Chinese little misery is the norm.
:
:
in the past where I recall contributors talking about thousands of an inch and only possessing rulers and lathes without dials and TPI which would only produce 62.5 gradations per revolution.

I feel sorry for those who are trying hard in solving the problems of their own little world of making models and things to go with them.
Hi Norman,

Please don’t confuse the issue by dragging “reality” and common sense in to the debate

My first two steam engines were to designs by LBSC and dimensional tolerances were defined in instructions to turn a part to “1/8 inch bare” or “1/8 inch full”

Ian
 

goldstar31

Well-Known Member
Joined
Feb 20, 2010
Messages
2,786
Reaction score
864
Location
Twixt Tyne and Tees
Hi Norman,

Please don’t confuse the issue by dragging “reality” and common sense in to the debate

My first two steam engines were to designs by LBSC and dimensional tolerances were defined in instructions to turn a part to “1/8 inch bare” or “1/8 inch full”

Ian
I was brought up in the. days when a blacksmith farrier had two pockets sewn into his fustians. One was for his best brass folding ruler and the other was one was worn with rounded ends from years of 'marking off' on metal. The rougher metal was marked off with regulation French chalk stick---- and it all worked.
It all worked as it did for his father before him in Shildon Works.

As for 'bare' and 'full', I never quite understood what LBSC was blethering about. I suppose it was some strange Masonic symbolism that despite being a Provincial officer, I have yet to be 'introduced'

We come to the seemingly forgotten part of our hobby and some seem to have forgotten that we don not work in a factory where some geyser llike me came around taking samples to see that the machines are endlessly producing stuff that lies within the 3 Standard Deviations of the Accepted Mean- or NOT!

We are making a one off which will hopefully fit or rattles. Surprisingly, it seems that a full size steam locomotive works best- when it rattles.

Probably, I'm missing those days when the designs were sketched out in the soil of the blacksmith's shop----------- and everything worked.

So you you have the practical experiences of a 90 year old whose IQ is certainly not lying - one the Mean but seems to have wondered off to 135------and seems to have worked enough not to be an engineer but to have successfully retired - for longer than I have ever worked.

I suppose that this is a test which few dare take

My thoughts, of course

Norman
 

Richard Hed

Well-Known Member
Joined
Nov 23, 2018
Messages
445
Reaction score
107
Location
Seattle
Hi Richard. Mostly, I was railing against the suggestion that "Don't overdimension a drawing is a useless holdover from the days of manual drafting", and that since "computers don't make drafting errors", this convention was now irrelevant. I'm sure you are already familiar with the issues, but there are so many self-taught/only-ever-driven CAD jockeys that think that this is true, that I believe this bears being explicit about.

While computers can be reasonably argued to make far fewer simple math errors than human draftspersons, the prohibition against overdimensioning was only ever peripherally about _mistakes_.

It was (and is) much more about preventing the possibility of a feature being able to be interpreted as located at more than one location, or having more than one dimension, with the difference depending on the path one takes through the provided dimensions. Even without mistakes, this can easily happen due to "invisible digits" that can creep into dimensions, most obviously as a result of trig relationships defining the position of features. The good designer or draftsperson makes sure that only those dimensions that allow the machinist to correctly position or dimension the part, are represented on the specification drawing.

Now, the wonder of the enabling technology of the computer doing the math for me to calculate derived dimensions to help me work through my machining strategy without needing to spend hours with a calculator, or a designer providing process hints like William May's "plunge your countersink .063 inches", those kinds of benefits I'll take any day of the week. I just wish more of today's designers and CAD jockeys understood that just because "the computer doesn't make math errors", doesn't suddenly make overdimensioning ok, or reduce the amount of thought that the designer needs to put into choosing how to dimension the features to correctly communicate the design intent!
Oh, yes, I agree. I thimk maybe that the "associations" who make those conventions should reconsider some things (maybe they already have and I just doesn't know it)--those things are not the dimensions themselves but rather a method to point out where the first datum point is, for instance, labeling it "A" (or what ever) and if there is a second datum to label it "B" and so on. There certainly are some symbols that could be used like this. Maybe already done and I just doesn't know it.
 

easymike29

Member
Joined
Jan 9, 2013
Messages
22
Reaction score
11
Location
San Diego CA
I mean no disrespect to any reader of this thread especially of the OP, but any of my apprentices could tell you the depth of that countersink. Most of them could derive it without picking up a pencil, just their calculator. The others would be able to sketch it out and then do the math. No muss, no fuss, no whining. They also would know that it only is of value as an approximation of how deep to plunge the countersink. He/she would only be concerned with thru hole size, countersink degrees and .225 Diameter at the opening. That's not all they were able to accomplish but what they did learn made them more valuable to a future employer. Don't underestimate what a competent machinist is capable of doing. Just create a properly toleranced object and don't be concerned about how he/she proceeds.
Please, readers, I am not posting this to offend anyone. If machining is just your hobby you can't or shouldn't be expected to have the knowledge of one that does it for a living.
The OP has asked for us to share some of that storehouse and has, I think, been adequately supplied with several suggestions. He is welcome to choose among them.

Eugene
 

easymike29

Member
Joined
Jan 9, 2013
Messages
22
Reaction score
11
Location
San Diego CA
For the benefit of math challenged and anyone else interested I have prepared a spreadsheet to calculate that .0627 dimension as well as 2 different ways to measure the mouth diameter. If anyone is interested I'll attach it in my next post.

Eugene
 

IanN

Well-Known Member
Joined
Aug 16, 2007
Messages
130
Reaction score
48
Location
Bath, UK
Hi Richard. Mostly, I was railing against the suggestion that "Don't overdimension a drawing is a useless holdover from the days of manual drafting", and that since "computers don't make drafting errors", this convention was now irrelevant. I'm sure you are already familiar with the issues, but there are so many self-taught/only-ever-driven CAD jockeys that think that this is true, that I believe this bears being explicit about.

While computers can be reasonably argued to make far fewer simple math errors than human draftspersons, the prohibition against overdimensioning was only ever peripherally about _mistakes_.

It was (and is) much more about preventing the possibility of a feature being able to be interpreted as located at more than one location, or having more than one dimension, with the difference depending on the path one takes through the provided dimensions. Even without mistakes, this can easily happen due to "invisible digits" that can creep into dimensions, most obviously as a result of trig relationships defining the position of features. The good designer or draftsperson makes sure that only those dimensions that allow the machinist to correctly position or dimension the part, are represented on the specification drawing.

Now, the wonder of the enabling technology of the computer doing the math for me to calculate derived dimensions to help me work through my machining strategy without needing to spend hours with a calculator, or a designer providing process hints like William May's "plunge your countersink .063 inches", those kinds of benefits I'll take any day of the week. I just wish more of today's designers and CAD jockeys understood that just because "the computer doesn't make math errors", doesn't suddenly make overdimensioning ok, or reduce the amount of thought that the designer needs to put into choosing how to dimension the features to correctly communicate the design intent!
Hi Willray,

I agree with your comments but would add that the true, practical, reason for not “over dimensioning” is the tolerance problem:

Imagine a 100mm +/- 0.1mm long item with a hole 20mm +/- 0.1mm form one end - what is the “missing” 80mm dimension tolerance?

Ian
 

Latest posts

Top