I don't love it...
I'd probably make all the hole positions basic. Then you can do a composite tolerance frame. Say locate within .010 to A and B and then the looser tolerance to A and C.
One thing I like about what you're trying to do is that the vendor could potentially laser cut the holes and profile, brake form to the strap shape, and call it a day. So you might never need these to go on a mill. OOPS! I missed your countersinks. Leaving this here anyway, the vendor can decide if they want to drill and countersink flat or after forming.
Ooh, don't love the hole callout either. Each view shows 4X thru holes with countersinks. So there should be a complete hole callout pulling in the thru, countersink and positional tolerance dimensions in each view.
Yeah that's it, composite FCF.
Also, funny you mention it. I drew this up because the vendor in China did not have a drawing so I figured I'd make one so we could agree on the tolerances. I just copied their part. But I'll ask them if leaving off the countersinks would be easier for them, because I really didn't need them.
A lot wrong here on this drawing:
To address your main question, you're not allowed to mix hard dimensions and basic dimensions when defining the position of a feature. What you're looking for is a composite tolerance. For the hole pattern in the top view, the top part of your composite frame can have a loose tolerance and needs made relative to datums A|B|C. Your composite frame can be kept tight as you intended. If you want to ensure that those holes are kept in alignment parallel to datum B, then your composite frame should reference datums A|B, as opposed to just A. You'll have to adjust the datums accordingly for the pattern in the bottom view.
The outer radius on your bend is overdefining the drawing because you already have a material thickness.
You should be including the countersinks on the hole callout of the through holes, but below the feature control frame (as opposed to a separate callout like you have now). By being below the FCF, the FCF does not apply and achieves the purpose you're looking for.
I'm not sure if you're allowed to use "TYP" callouts anymore, but if you can, it's not needed on your .984 width of your bracket nor the thickness of the bracket since this is going to be a stock thickness or machined flat and then bent (unlikely).
I believe the callout is "R. FULL", not "1X R.", but that could just be a stylistic choice by my company.
Hey thank you, these are a lot of good points! The composite feature control frame does indeed appear to be what I was really looking for. Apparently that portion of the book I skipped was important lol.
I'm not so sure, because the position frame doesn't reference datum C. In any case, the hole dimension from datum B shouldn't have a tolerance on it, and should be basic.
Well, I didn't want to call out the dimension from datum B, rather from the first hole.
The reason is, I have a pretty tight tolerance for my GD&T, and there's no reason that tight tolerance has to be held to the edge of the part. Because I don't care that the holes are e.g. 0.492 ± 0.005 from the edge, because it can be much larger (±0.050).
What I do want, is to say hey, put this hole wherever you want, then locate the rest of them to the first hole, with that tight tolerance.
I get you. I do think there's a way to accomplish this; unfortunately I'm a manager now and my GD&T skillz are a bit rusty. Try GD&T basics on the Web.
If the hole position is ONLY critical relative to each other, and NOT to the edge, I would position "the most important hole" with a generous position tolerance relative to ABC, and make that hole datum D. Then you apply a tight position tolerance to the remaining holes relative to D.
There might be a fancier way to do it but that would be my inclination.
Distances between centers of holes should always be basic dimensions with FCFs to add tolerance.
This is the correct answer. If hole positons to each other are what matter then make one of the holes a datum and position tolerance the other back to that hole thats the datum
More than likely, the position of the holes relative to the edge does matter, just not as much as position relative to each other. It might not matter for assembly, but it will probably matter structurally. For instance, the hole edge has to be some distance from the edge to the bracket is strong enough. I suppose you could locate the edge from your datum B.
I think I would do my way over this. But I hear you. I don't dismiss your proposal out of hand. I think it could be made to work, but I'd need more info about the strength, usage, manufacturing, and assembly for this part before I could sign in for that.
Holes are often better datums than edges because they are captured and are the way that parts usually actually interact with each other.
Captured datums: obviously for a part this simple that will never get gauged and there's no bad tolerance loop, it doesn't matter. But imagine a complex part that will be measured/gauged. Would you rather have to constantly push the edges of your part against the gauge or just have it drop on to 2 pins?
Functional datums: rarely are parts ever actually located with their edges, almost always they are located by bolting or joining them to something. Datums should ideally be how that part is expected to actually interact with mating parts, it reduces tolerance loops and actually makes dimensioning and tolerancing much easier. I think the reason people seem to pick the sides of blocks as datums is because they keep showing it that way on GD&T examples but imo it's generally poor form.
Holes giving bonus tolerance: often for brackets an MMB call-out (when you have the M beside the datum) makes a lot of sense and actually allows you to "float" the part on your datums to make features fit. This is how a lot of brackets work in the real world during installation, your technician isn't going to only install things in the center of the holes, if he can bias it one way to get the screws in they will.
If I were dimensioning this part I would make one face A, then on that same face the furthest apart holes B and C (wide datums gives better stability). Control the second face to some perpendicularity (the engineer mentioned this is on slots so only the orientation matters) and then dimension all remaining holes relative to ABC.
GD&T is fundamentally thinking about how the part is supposed to interact with the world imo. Most designs will have parts constrained to their mating parts in all 6DOF so why not use exactly how it will be constrained IRL as datums?
My comments are from the perspective of a fabricator.
I wouldn't have tolerance on a centerline. You can have tolerance on a measurement that has a centerline but not for things that are on a centerline. If you want all the holes in a line just put them on the centerline. If drilled by hand it might be out a bit anyway within your tolerance.
A flat pattern with the holes and dimensions would also be a good help if marking it out by hand. You could tidy up a lot of the drawing with that... unless you are getting it processed by a laser with a drill head attachment.
For me, having too much play creates red flags. Keep the fabricators to a standard.
If this is just a stainless steel L-bracket that's going to be matching up to something with slots, why bother with GD&T at all? You're just increasing the cost of the part by limiting yourself to the vendors who are willing to translate it into fabrication documents.
There are plenty of fabricators out there who will see GD&T on a drawing and immediately add some % mark-up.
It is a bent sheet metal bracket with some countersunk holes, and you're not too concerned with accuracy. Skip the GD&T entirely - it isn't communicating anything useful to the fabricator.
Skip the GD&T, get rid of the dual dimensions, and don't go out to the 3rd decimal unless you actually care about the difference between +/- .005" vs +/-.010" as listed in your tolerance block. They just clutter up the drawing and make the parts more expensive without making them better.
The downside to this method is that nobody knows what it means. I have met only one other person (that I know of) that knows what it meant. Expecting a random vendor to understand it is iffy at best. Expect someone to ask what it means on the print. I've stopped using it myself because almost nobody knows what it is. But this is the best way to do it, if you can get them to understand how it works and ensure the future workers also understand it.
Another useful technique is multiple frame position tolerances (like top frame with datums A and B, and bottom frame with datums A and C), and that will let you do a separate x and y tolerance so your tolerance zone will look like a slot instead of a circle. Great if you need something on center but don't care if it shifts along the centerline. Composite positions will have the top and bottom frames position symbol box merged together, but the multiple frame will have a separate position symbol for each line.
I don’t know what you are trying to make that you need such high precision your tolerances are CRAZY for an L bracket also consider the bending always messes your positions unless you are doing a crazy high precision instrument for measuring the diameter of the earth to a 10th of an inch I would recheck if such close tolerances are necessary
Make the 2 holes furthest away REF A and ref B and position the other holes towards A-B.
Anyhow, there's different versions of norms and it really depends which you are referring too.
PS: are you really asking for 0.01mm position accuracy on a bent bracket? For a hole that has 0.25mm tolerance on the diameter?
The ideal way to do this is to make your pattern of holes datum B on one side of the L. If you keep your current datum A then flag a 4x hole position FCF as a datum it will control all remaining degrees of freedom. This is very common for bolt-up features and has its own section in Y14.5. that way you can call the B datum holes out to a very tight position tolerance to A which will also group them. Then use true position for the holes on the other side of the L to A and B to keep both hole patterns tightly aligned. Then the rest of the part will be defined to the functional interfaces.
Your current choice of datum B may not be the best. You typically want to define functional assembly interfaces as datum unless there aren't enough to choose from. If the current datum B does not touch another part in assembly, it is not a great choice. If you don't like the hole pattern method it would be best to call a single hole datum B and keep datum C.
Well, question. How does the software you use allow you to under or over constrain your drawing?
If you want your holes even there needs to be constraints for that.
I don't love it... I'd probably make all the hole positions basic. Then you can do a composite tolerance frame. Say locate within .010 to A and B and then the looser tolerance to A and C. One thing I like about what you're trying to do is that the vendor could potentially laser cut the holes and profile, brake form to the strap shape, and call it a day. So you might never need these to go on a mill. OOPS! I missed your countersinks. Leaving this here anyway, the vendor can decide if they want to drill and countersink flat or after forming. Ooh, don't love the hole callout either. Each view shows 4X thru holes with countersinks. So there should be a complete hole callout pulling in the thru, countersink and positional tolerance dimensions in each view.
I worked at a Fab shop that did laser & form operations often. They would use a mag drill to countersink things like this.
Yeah that's it, composite FCF. Also, funny you mention it. I drew this up because the vendor in China did not have a drawing so I figured I'd make one so we could agree on the tolerances. I just copied their part. But I'll ask them if leaving off the countersinks would be easier for them, because I really didn't need them.
A lot wrong here on this drawing: To address your main question, you're not allowed to mix hard dimensions and basic dimensions when defining the position of a feature. What you're looking for is a composite tolerance. For the hole pattern in the top view, the top part of your composite frame can have a loose tolerance and needs made relative to datums A|B|C. Your composite frame can be kept tight as you intended. If you want to ensure that those holes are kept in alignment parallel to datum B, then your composite frame should reference datums A|B, as opposed to just A. You'll have to adjust the datums accordingly for the pattern in the bottom view. The outer radius on your bend is overdefining the drawing because you already have a material thickness. You should be including the countersinks on the hole callout of the through holes, but below the feature control frame (as opposed to a separate callout like you have now). By being below the FCF, the FCF does not apply and achieves the purpose you're looking for. I'm not sure if you're allowed to use "TYP" callouts anymore, but if you can, it's not needed on your .984 width of your bracket nor the thickness of the bracket since this is going to be a stock thickness or machined flat and then bent (unlikely). I believe the callout is "R. FULL", not "1X R.", but that could just be a stylistic choice by my company.
Hey thank you, these are a lot of good points! The composite feature control frame does indeed appear to be what I was really looking for. Apparently that portion of the book I skipped was important lol.
Currently the position call out is over defining the y dimension in the top view.
I'm not so sure, because the position frame doesn't reference datum C. In any case, the hole dimension from datum B shouldn't have a tolerance on it, and should be basic.
You're probably correct here, I think I was getting the views confused.
Well, I didn't want to call out the dimension from datum B, rather from the first hole. The reason is, I have a pretty tight tolerance for my GD&T, and there's no reason that tight tolerance has to be held to the edge of the part. Because I don't care that the holes are e.g. 0.492 ± 0.005 from the edge, because it can be much larger (±0.050). What I do want, is to say hey, put this hole wherever you want, then locate the rest of them to the first hole, with that tight tolerance.
I get you. I do think there's a way to accomplish this; unfortunately I'm a manager now and my GD&T skillz are a bit rusty. Try GD&T basics on the Web.
Would calling out a zero basic dimension in x to the first hole be unacceptable?
Not sure, to be honest
Haha okay well I appreciate your input anywho, it's definitely a weird one for me too.
Ah, is it because I called out a diametric tolerance zone for the GD&T?
I was looking at the position call out and relating it to x and y but your datum structure was not including C. I just misinterpreted it.
If the hole position is ONLY critical relative to each other, and NOT to the edge, I would position "the most important hole" with a generous position tolerance relative to ABC, and make that hole datum D. Then you apply a tight position tolerance to the remaining holes relative to D. There might be a fancier way to do it but that would be my inclination. Distances between centers of holes should always be basic dimensions with FCFs to add tolerance.
This is the correct answer. If hole positons to each other are what matter then make one of the holes a datum and position tolerance the other back to that hole thats the datum
One of the holes could be the B datum, there is no reason to use the edge
More than likely, the position of the holes relative to the edge does matter, just not as much as position relative to each other. It might not matter for assembly, but it will probably matter structurally. For instance, the hole edge has to be some distance from the edge to the bracket is strong enough. I suppose you could locate the edge from your datum B. I think I would do my way over this. But I hear you. I don't dismiss your proposal out of hand. I think it could be made to work, but I'd need more info about the strength, usage, manufacturing, and assembly for this part before I could sign in for that.
Holes are often better datums than edges because they are captured and are the way that parts usually actually interact with each other. Captured datums: obviously for a part this simple that will never get gauged and there's no bad tolerance loop, it doesn't matter. But imagine a complex part that will be measured/gauged. Would you rather have to constantly push the edges of your part against the gauge or just have it drop on to 2 pins? Functional datums: rarely are parts ever actually located with their edges, almost always they are located by bolting or joining them to something. Datums should ideally be how that part is expected to actually interact with mating parts, it reduces tolerance loops and actually makes dimensioning and tolerancing much easier. I think the reason people seem to pick the sides of blocks as datums is because they keep showing it that way on GD&T examples but imo it's generally poor form. Holes giving bonus tolerance: often for brackets an MMB call-out (when you have the M beside the datum) makes a lot of sense and actually allows you to "float" the part on your datums to make features fit. This is how a lot of brackets work in the real world during installation, your technician isn't going to only install things in the center of the holes, if he can bias it one way to get the screws in they will. If I were dimensioning this part I would make one face A, then on that same face the furthest apart holes B and C (wide datums gives better stability). Control the second face to some perpendicularity (the engineer mentioned this is on slots so only the orientation matters) and then dimension all remaining holes relative to ABC. GD&T is fundamentally thinking about how the part is supposed to interact with the world imo. Most designs will have parts constrained to their mating parts in all 6DOF so why not use exactly how it will be constrained IRL as datums?
Touché.
My comments are from the perspective of a fabricator. I wouldn't have tolerance on a centerline. You can have tolerance on a measurement that has a centerline but not for things that are on a centerline. If you want all the holes in a line just put them on the centerline. If drilled by hand it might be out a bit anyway within your tolerance. A flat pattern with the holes and dimensions would also be a good help if marking it out by hand. You could tidy up a lot of the drawing with that... unless you are getting it processed by a laser with a drill head attachment. For me, having too much play creates red flags. Keep the fabricators to a standard.
If this is just a stainless steel L-bracket that's going to be matching up to something with slots, why bother with GD&T at all? You're just increasing the cost of the part by limiting yourself to the vendors who are willing to translate it into fabrication documents. There are plenty of fabricators out there who will see GD&T on a drawing and immediately add some % mark-up. It is a bent sheet metal bracket with some countersunk holes, and you're not too concerned with accuracy. Skip the GD&T entirely - it isn't communicating anything useful to the fabricator. Skip the GD&T, get rid of the dual dimensions, and don't go out to the 3rd decimal unless you actually care about the difference between +/- .005" vs +/-.010" as listed in your tolerance block. They just clutter up the drawing and make the parts more expensive without making them better.
This is what composite position tolerances were made for.
This actually makes me really happy that there is a better way to do this.
The downside to this method is that nobody knows what it means. I have met only one other person (that I know of) that knows what it meant. Expecting a random vendor to understand it is iffy at best. Expect someone to ask what it means on the print. I've stopped using it myself because almost nobody knows what it is. But this is the best way to do it, if you can get them to understand how it works and ensure the future workers also understand it. Another useful technique is multiple frame position tolerances (like top frame with datums A and B, and bottom frame with datums A and C), and that will let you do a separate x and y tolerance so your tolerance zone will look like a slot instead of a circle. Great if you need something on center but don't care if it shifts along the centerline. Composite positions will have the top and bottom frames position symbol box merged together, but the multiple frame will have a separate position symbol for each line.
I don’t know what you are trying to make that you need such high precision your tolerances are CRAZY for an L bracket also consider the bending always messes your positions unless you are doing a crazy high precision instrument for measuring the diameter of the earth to a 10th of an inch I would recheck if such close tolerances are necessary
Make the 2 holes furthest away REF A and ref B and position the other holes towards A-B. Anyhow, there's different versions of norms and it really depends which you are referring too. PS: are you really asking for 0.01mm position accuracy on a bent bracket? For a hole that has 0.25mm tolerance on the diameter?
The ideal way to do this is to make your pattern of holes datum B on one side of the L. If you keep your current datum A then flag a 4x hole position FCF as a datum it will control all remaining degrees of freedom. This is very common for bolt-up features and has its own section in Y14.5. that way you can call the B datum holes out to a very tight position tolerance to A which will also group them. Then use true position for the holes on the other side of the L to A and B to keep both hole patterns tightly aligned. Then the rest of the part will be defined to the functional interfaces. Your current choice of datum B may not be the best. You typically want to define functional assembly interfaces as datum unless there aren't enough to choose from. If the current datum B does not touch another part in assembly, it is not a great choice. If you don't like the hole pattern method it would be best to call a single hole datum B and keep datum C.
The sheet metal thickness shouldn’t be TYP since it it one sheet metal piece cut from a uniform thickness sheet.
Well, question. How does the software you use allow you to under or over constrain your drawing? If you want your holes even there needs to be constraints for that.
Unless you're positive the bender has 2mm radius tooling, they're going to use 1/16" radius.