I haven't really had to use geometric tolerancing for a few years and I am a little bit out of touch.

 

We have a part that is constantly coming in from our supplier with the mount holes misaligned (slots in the mount tabs). The slot locations are relative to the location of the main connection point - which is the 4" NPT shown on the drawing below. This part mounts to the legs of a C12 channel (legs facing the part) - there is a larger hole for the 4" NPT to fit through on the inside face of the channel.

Note that I have applied a 0.03 (1/32") parallel geometric tolerance, to both legs of the mount bracket, in relation to the center line of the 4" NPT connection. If memory serves me correctly, this could lead to a max of 1/16" tolerance on the slot alignment - please correct me if I am wrong with that.

If that is the case, I am OK with that because the ones we have been receiving have been a full hole diameter(+) off - as in, you could get bolt #1 in, but couldn't see the hole at all on the other side for bolt #2.

 

This unit is supplied to us from a 2nd party manufacturer. This is their own design - meaning we did not do any of the manufacturing drawings for this unit or any of it's pieces. I created this drawing just so that we could make sure that we stay on the same page with the manufacturer and they know what we are expecting to receive from them. With that information, I did do a REFERENCE design for the mounting band (the part with the slots) that is included with this drawing on the second page.

 

Our speculation is that, whenever the mfr. rolls the center part of this bracket, they, somehow or another, twist the piece - so that the slots no longer line up. I created the reference drawing just to drive home the point that we want these legs parallel - or at least, we want the holes to line up as close as possible. Here is the detail on the second page:

My questions are:

1) Is the geometric tolerancing on the second page superfluous?

2) Will my .03 variance on each page combine to allow a greater/looser tolerance than what I am after in the assembly? My gut tells me NO, because, regardless of the second GDT, the assembly tolerance holds priority.

 

Thoughts??


Categories: General

Comments
Last comment By: Scott Casale   Fri, 13 Oct 2017 20:42:49 GMT
Re: Geometric Tolerance - a second opinion

In my opinion the true position of the slot(s) relative to the npt fitting is an issue more so than the legs actually being parallel?  Also that NPt fitting has no location data to it's "horizontal" position. That 9.63" measurement has an associated tolerance, what is it? +/- 0.01"?

By: Christopher Culver  Thu, 12 Oct 2017 16:10:43 GMT
Re: Geometric Tolerance - a second opinion

It's best to think of this with the mindset of "how would I fixture this to measure the slots with respect to the hole?"

 

Datum A should be preferably a flat or easily controllable surface on which to lay the part. It appears as if the only flat on this part is the face of the bent mounting bracket. You'll want to essentially constrain the parallel flanges and the NPT Axis together. I'm a bit rusty on this so don't take my opinion as anything other than just that. I think basic dimensions can be used when calling out the 9.63 dimension because the GD&T controls the tolerance zone of that part.

 

I'm sure more would be needed but this is just a quick swag. The idea is to make the NPT fitting perpendicular to A, which is flat. C is perpendicular to A as well, referencing B which ties those together more or less as parallel with one another. You will just need to note perhaps with another datum that the other flange opposite C is controlled.

 

By: Alex Burnett  Thu, 12 Oct 2017 16:32:07 GMT
Re: Geometric Tolerance - a second opinion

I have got to go back and make some repairs to this sheet - for some reason, the changes didn't hold and the file went corrupt.

 

But, to answer your question(s):

Yes, the crucial tolerance is that which associates the center of the slots to the center line of the 4" NPT.

The location of the 4" NPT is locked in a different view - I will display full sheet after correcting the issues.

The 9.63 dimension is shown as a "check" dimension for our quality control engineer. This just signifies that he needs to verify this dimension is within the specified tolerance - a "crucial" dimension if you will.

 

**Drawing Fixed**

Note that the 4" NPT is located by A and B and the bracket is located reference from that. (I don't know why the .75 is showing orange - I think it highlighted as I was choosing the window).

 

The .01" tolerance was put on by the previous designer - I am just modifying this sheet with new dimensions and GDT. I will probably go back in and change that to .03" (1/32")

By: Kevin Andrews  Thu, 12 Oct 2017 16:38:36 GMT
Re: Geometric Tolerance - a second opinion

Hello,

 

I don't believe the parallel helps with your positioning.

Even when satisfied, parallel won't hold either left/right or up/down.

As long as the vertical slot axes are parallel to A, then each slot can float independently of the other.

 

Just a quick look, I hope it helps.

 

Kevin C.

By: Kevin Chandler  Thu, 12 Oct 2017 16:56:49 GMT
Re: Geometric Tolerance - a second opinion

If the 9.63 +/- .03(I think +/- .01 will be better as this is critical) dimension is held, that location can vary from 9.60-9.66 from the centerline of the fitting, the parallel callout only constrains the centerline axis of the slots, so they can not be skewed from the centerline of the fitting, that does not constrain any part of the slot location beyond the above which takes precedence. The slot is .680" wide(+/-?? tolerance), using 5/8" hardware? That leaves .0275" per fore/aft at nominal of clearance if so. What are the tolerances of the features in the channel that this assembly mates to? I think the parallel call-out is unnecessary, and you need the constrain the slots relative to the fitting, not the actual bracket itself.

 

For assembly my fixture would do exactly that, bolt bracket to c-channel fixture, place vessel and fitting center within the hole in c-channel, and affix bracket to cylinder. 

By: Christopher Culver  Thu, 12 Oct 2017 18:06:10 GMT
Re: Geometric Tolerance - a second opinion

I think you are missing a step - but I may be wrong...in order for all of your steps to work, I would also need to apply a "straightness" GDT to the horizontal center line (hence the statement of C & B being perpendicular to A. I could also add a datum to the callout itself for reference to other GDT...for conversation sake, lets call this datum "Z".

Let me rethink this and see if I can fix this and go from here...I believe this thread will serve as a decent learning tool for some - including me.

By: Kevin Andrews  Thu, 12 Oct 2017 18:17:59 GMT
Re: Geometric Tolerance - a second opinion

You are absolutely right in your assessment that the parallel GDT would not achieve what I was looking for....it would, as far as keeping the centers of the slots parallel to A - but it does nothing for the placement of the slots (location from A). By the GDT listed, the slots could be out of alignment by inches and still hold true to the parallel of A.

 

To you sir, a badge and 10 points...I can't call correct answer because you only pointed out the issue without further resolution (not meant to be an ass-remark) - I hope you understand.

 

Stay tuned as I am taking everything in and will revamp the drawing shortly.

By: Kevin Andrews  Thu, 12 Oct 2017 18:27:59 GMT
Re: Geometric Tolerance - a second opinion

Parallelism does not control position.  It only controls orientation and flatness.

 

You need to get rid of the parallelism make the 9.63 dimension basic and add a single direction position tolerance to the slot itself.

 

Something like this:

 

Even here, this is the wrong callout:

 

Make the centerline of one the datum (you have that), and then create a position tolerance.  Flatness and parallelism can "float" inside the linear tolerance zones on your dimensions.

By: Dan Pihlaja  Thu, 12 Oct 2017 18:36:28 GMT
Re: Geometric Tolerance - a second opinion

Hello,

 

Thank you for the badge!

 

I think a positional tolerance on the 9.63 inspection dim is required.

Also, since A is an axis, 2 planes are established by designating it as a datum, so the parallel to B should be to A only.

A & B share a common plane (along the long axis on the cropped view) and only differ on when square to the cropped view.

So the parallel to B also references A (and should be positional).

 

Position will locate and hold parallel on the side view because you're referencing the slot vertical axis.

 

I hope this helps,

 

Kevin C.

By: Kevin Chandler  Thu, 12 Oct 2017 18:37:06 GMT
Re: Geometric Tolerance - a second opinion

You are also getting a badge and 10 points because you seem to have put in a lot of thought to this one - or maybe it just comes naturally...either way, it is deserving and is making me think everything through.

 

In response to your comments though:

Your first paragraph is 90% correct. Personally, I feel the .01 tolerance is a bit much and I will probably increase that some. The channel, however, will be an all-together different animal to go back and look at.. - which I will do when I finish this drawing.

 

Your second paragraph would be, almost, optimal with the exception of one thing: two different suppliers

We receive the tanks prefabricated from the supplier - with mount bracket already welded to the body. The channel mounts come from a different supplier & they are dissimilar materials (the tank comes in powdercoated steel and in stainless)...

 

I think I have a good amount of information to build on..let me see what I can come up with now. Will post again in a few.

By: Kevin Andrews  Thu, 12 Oct 2017 18:39:34 GMT
Re: Geometric Tolerance - a second opinion

adding more GDT to the part will increase the cost. you might be better off drilling the holes in house. just have the channel made with the 4 inch hole.

By: Scott Cole  Thu, 12 Oct 2017 20:16:19 GMT
Re: Geometric Tolerance - a second opinion

OK - Thank you to all who have responded and tuned in to see what became of this. I believe I have taken a little bit of everybody's suggestions and incorporated them into this final drawing. Minus one last question, I believe I have this constrained as much as possible.

Here is what it looks like now:

Lower Left View:

So, datum "A" is now my center line through the body. I did not need to add any GDT to this because it will always be in the center of all directions relative to the body itself. I considered using a "straightness" GDT, but decided that it really didn't need it.

 

I set the center line of the 4" NPT as datum "B" and GDT'd the center line "perp" to "A".

 

 

I dimensioned to the center point of the slot so that I could add two GDTs for correct location. I used a "position" GDT on the callout for the size of the slot - relative to "A" and "B". This shoulod accurately place the slot where I need it. I also set the center line of the slot "perp" to "A" so that the slot would truly run perpendicular to "B". I also added a reference dimension on the slot so that there would be no question about the slot callout.

**Since this picture was taken, I also added the words "EACH SIDE" under both GDT callouts for the slot**

 

Any dimension with an oval/slot around the dimension is an inspection dimension and is just notation for the QA engineer in the warehouse. Note that both center point dimensions for the slot are labeled as inspection dimensions. Any dimension that does not have a GDT should follow the sheet tolerance of +/- .02" (I changed this from .01 as well). For the record, the 5.88 dimension is not that critical, so long as the 9.63 is correct.

 

I also cleaned up some of the dimensions in this view because it was just too busy..

 

Lower Right View:

I moved some of the excess dimensions from the lower left view to this view. I also referenced the center line of the body as "A" again.

I then added a "perp" GDT to the center line of the 2" NPT half-coupling and gave a center line dimension as well.

I also called out the overall leg length of the bracket (3.54).

 

Upper Right View:

I noted datum "B" as it will be referenced in this view. I then added the angular dimension to show that the 2" NPT coupling should be 180° from the 4" NPT. I also applied an angularity GDT to "B" here.

 

Then, I added the "parallel" GDT to each leg of the bracket.

 

Upper Left View:

This one, I really just cleaned up any superfluous dimensions and made it look better.

 

NOW, my (hopefully) last question:

The tolerance listed for "amgularity",  "perpendicular" and "parallel" GDT.....isn't that based on degrees vs. linear? So, my tolerances should be +/- 0.10° of 90° or 180°....Just making sure.

 

Again, thank you to all who have contributed.

By: Kevin Andrews  Thu, 12 Oct 2017 20:21:50 GMT
Re: Geometric Tolerance - a second opinion

Compared to the headaches this has caused in the field...I think I will be OK. All of the GDT are strictly used to accurately locate the mount holes to the center of the 4" NPT. I am aware that this could cause excess costing, but.....it is a necessity.

By: Kevin Andrews  Thu, 12 Oct 2017 20:24:39 GMT
Re: Geometric Tolerance - a second opinion

Hello,

 

The 180° dim (actually it's two of the 90° quadrant angles) are implied, so the 180° should be reference dim.

The angularity to B is fine.

 

Also, as I stated above, axis datums generate implied cross planes, so parallel .01 to B is can be to A.

 

Also, there's no reference to the far slot.

 

Kevin C.

By: Kevin Chandler  Thu, 12 Oct 2017 20:34:35 GMT
Re: Geometric Tolerance - a second opinion

I ended up taking out the angularity tolerance for the 2" NPT (the 180°) - I just didn't come back and say anything as I feel y'all are getting pretty tired of me at this point...

 

I understand about the cross planes, but I needed the datum "B" to be able to give an accurate position GDT for the slot location. I figured that, since it was there, I might as well use it (for the parallel GDT in the upper right) to help alleviate any confusion in the shop.

 

The "far slot" is noted with a callout of "EACH SIDE" under the GDT callouts for the slot. I just hadn't added them before I posted that picture:

By: Kevin Andrews  Thu, 12 Oct 2017 20:47:15 GMT
Re: Geometric Tolerance - a second opinion

Kevin Andrews wrote:

 

I ended up taking out the angularity tolerance for the 2" NPT (the 180°) - I just didn't come back and say anything as I feel y'all are getting pretty tired of me at this point...

 

I understand about the cross planes, but I needed the datum "B" to be able to give an accurate position GDT for the slot location. I figured that, since it was there, I might as well use it (for the parallel GDT in the upper right) to help alleviate any confusion in the shop.

 

The "far slot" is noted with a callout of "EACH SIDE" under the GDT callouts for the slot. I just hadn't added them before I posted that picture:

 

You can't call out your position tolerance like that.  If you don't have the diameter symbol, then you need to give it a direction.

Does it apply to the vertical direction or the horizontal direction?

The best way (in my opinion) is to add a horizontal dimension to the width of the slot and add the positional tolerance to it.  Then add the vertical dimension separately.  You can even add a separate positional tolerance to the vertical dimension and make it different.

By: Dan Pihlaja  Fri, 13 Oct 2017 11:51:29 GMT
Re: Geometric Tolerance - a second opinion

Correction - this tolerance means that it can move in a square (X & Y direction) +/- 0.01 in either direction. But still accurately places the location.

By: Kevin Andrews  Fri, 13 Oct 2017 12:39:43 GMT
Re: Geometric Tolerance - a second opinion

Myself being open minded, I am going to challenge you on this one - I may be wrong and I am fine with that if so. However, the position tolerance indicates that the center point of the feature has to be within a toleranced diameter of the basic dimension locations. For a position tolerance, two basic dimension, notating the center point of the feature, and two datum references are required.

There is nothing, that I have found, that says this tolerance ONLY applies to holes or circles - the symbol is not a diameter symbol either, so that does not apply. Granted, when referencing a center point, we most notably think of a round hole...but:

 

1) I have two basic dimensions applied to locate the center of the slot -

2) I have two datums referenced in both the X direction and the Y direction -

 

I also found a GDT tutorial from some school that I don't remember where it cmae from - I downloaded it yesterday. Here is the page where it explains the "position" GDT:

So, by definition, my position GDT simply states that the center point of the slot must be within a Ø.02 of where I have it located at through basic dimensioning. Which means it can only move .01 in any direction from where I have it called out at.

 

Also: https://www.gdandtbasics.com/true-position/  (last paragraph under final Notes)

By: Kevin Andrews  Fri, 13 Oct 2017 12:38:10 GMT
Re: Geometric Tolerance - a second opinion

Kevin Andrews wrote:

 

Myself being open minded, I am going to challenge you on this one - I may be wrong and I am fine with that if so. However, the position tolerance indicates that the center point of the feature has to be within a toleranced diameter of the basic dimension locations. For a position tolerance, two basic dimension, notating the center point of the feature, and two datum references are required.

There is nothing, that I have found, that says this tolerance ONLY applies to holes or circles - the symbol is not a diameter symbol either, so that does not apply. Granted, when referencing a center point, we most notably think of a round hole...but:

 

1) I have two basic dimensions applied to locate the center of the slot -

2) I have two datums referenced in both the X direction and the Y direction -

 

I also found a GDT tutorial from some school that I don't remember where it cmae from - I downloaded it yesterday. Here is the page where it explains the "position" GDT:

So, by definition, my position GDT simply states that the center point of the slot must be within a Ø.02 of where I have it located at through basic dimensioning. Which means it can only move .01 in any direction from where I have it called out at.

 

Also: https://www.gdandtbasics.com/true-position/ (last paragraph under final Notes)

Ok, I wasn't saying that the position is only applicable to cylinders.

 

What I was saying was that your intention isn't clear,

 

If you have the a dimension like this:

Then this means that the vertical center plane of the slot must fall between two perfect planes measuring .02" away from each other centered on the perfect theoretical centerline.

 

However, if you have it like this:

Then the problem is now that you are no longer controlling orientation of the slot.  This position now ONLY applies to the theoretical center POINT of the slot.  And you haven't indicated the shape of the tolerance.

If you want the tolerance zone to be square cylindrical, then you need to say it like this:

 

Now you have indicated the shape of the tolerance zone (cylinder).  If you want the tolerance zone to be square, then you can just use linear dimensions without a positional tolerance.

 

However the problem remains, that with this callout, the orientation of the slot is no longer controlled.

 

To control the orientation and position (specifically, vertically), then the callout needs to be:

I added the horizontal one just to show you how they can be different and still be legal.

By: Dan Pihlaja  Fri, 13 Oct 2017 15:12:41 GMT
Re: Geometric Tolerance - a second opinion

Just my 2 cents, but you keep trying to use imaginary lines as datum. Center-lines are not something a person on the shop floor can easily measure too, they are mainly used by drafters only. To get it really accurate the shop would make some sort of cylinder that fits inside the pipe or or slot, and then measure from a mark on that. And though the inserts may not be tightly fitting, it is much more accurate than trying to use a measuring tape and trying to eyeball where the center-line of a slot or pipe is. This problem doubles when you try to measure from one center-line to another center-line, even when using GDT. There is simply no hard surface that is really being measured off of, no edge that a measuring tape can hook onto.

 

What is probably causing some of your problems is that the manufacturers are just measuring to the edge of the slots, and trying to eye-ball the center-line of the pipe.

 

Have you considered making some sort of jig to send to these manufacturers to test the tolerance on the shop floor? A pair of jigs even, to test the minimum and maxim of tolerances.

By: Steven Mills  Fri, 13 Oct 2017 15:31:48 GMT
Re: Geometric Tolerance - a second opinion

Kevin,

 

Coming from a design field where 50% of my time is designing welding fixtures looking at your prints. I have an idea without the verbage of what you are looking for. Centerlines are ok to use as datums on welded structure as long as the expectation is a Faro arm is to be used for first article inspections. Along those same lines there will have to be a go no go jig built to validate all other parts. The other option is a fixture is built that passes first article inspection in free state. Or your print has to specify if the bracket is to be restrained.

 

I would say your best option for future control of this process is to build a jig for welding and a go no go gage for welding and inspecting this part. It would in the long run keep costs and rework down.

 

All of the tolerancing in the world will not fix the problem if there is an inherent flaw in the process.

 

I am going to assume that the shop that welds this has some sort of fixture already as free state welding it would be bothersome depending on the quantity. If they do ask to see it and see if there is something there you can work with to get a fixture that represents what you want to happen.

By: Paul Risley  Fri, 13 Oct 2017 16:08:03 GMT
Re: Geometric Tolerance - a second opinion

Hello,

 

Another item that may help is to eliminate the arc on the mount bracket and instead use tangent flats.

Even though it's narrow, straight bends are easy to replicate and are consistently held to the backstop.

And since it's mirrored, the part is swung around and bent the same (for each of the three backstop depths).

 

Back to the GD&T:

Place a positional tolerance on the vertical axis of the slot, but this must be without the diametral symbol before the tolerance value.

Without the diametral symbol, the vertical axis is restricted similar to a parallel (two limiting planes either side of theoretical slot vertical center), plus you get the location held as well (to the basic dim).

The vertical axis needn't be held as tight (it's a slot!), so a std dim (at default sheet tolerances, if close enough) is all that's required for vertical lopcation.

 

BTW:

In the attached "untitled.png" (stolen from a previous post above), I don't believe the diametral symbol is correct since the slot axis is indicated.

An axis can't "float" around in circular space since it doesn't have a point (the intersection of X-Y basic dims) to anchor it.

Omit the diametral symbol for this case and the form t is that the actual slot walls can vary (of any profile, for the slot depth) as long as the resultant centerline axial plane (for the entire slot length) remains within the two limiting planes (about the theoretical center axial plane) defined in the tolerance (and that any variance also doesn't violate the tolerance).

 

Cheers,

 

Kevin C.

By: Kevin Chandler  Fri, 13 Oct 2017 17:15:31 GMT
Re: Geometric Tolerance - a second opinion

So far, this has really been about trying to learn different methods of GDT and how I could apply it to my specific situation. My coworker was out yesterday, but I ran it by him this morning. He showed me that all of us were really over complicating it and he broke it down in to a few different reasons:

1) This "tank" comes from a third party vendor. We order it locally, but they receive it from, either, China or Japan (I think Japan). So, they will not try to hold our tolerance - at best, I may get 3/32" tolerance from them.

2) More than likely, they will probably ignore any GDT markings on the print - which makes them pointless anyhow.

 

The issue we have is that when they make the the bracket, they put it on a roller and roll the center section (the part that hugs the tank). If these rollers are not lined up perfectly, or the operator doesn't line everything up just right, it will cause the bracket to be twisted. Using the term loosely, we just want to convey that the slots should be concentric and perpendicular to the center line of the body...

 

After we tried wrapping our heads around the issue, it hit us smack in the face like a brick. I don't need GDT to get the point across. I just need a little more explanation on the print and I can use standard dimensioning with tolerance. This will also help to keep the cost from skyrocketing due to all the toleranced information.

 

I will post a new picture when I have it completed.

By: Kevin Andrews  Fri, 13 Oct 2017 18:24:55 GMT
Re: Geometric Tolerance - a second opinion

I agree.

By: Christopher Culver  Fri, 13 Oct 2017 18:30:57 GMT
Re: Geometric Tolerance - a second opinion

Has nothing to do with your drawing and how you should do it... but adding that type of tolerance on a pc that is hand rolled and air bent, that's a tough one and if it would have hit our shop years ago, the cost just went up and an additional tool would have been made at the welding station, a flat with a big old tenon and a clamp, which would be used to twist the bracket after it's welded... 

By: John Stoltzfus  Fri, 13 Oct 2017 18:54:39 GMT
Re: Geometric Tolerance - a second opinion

No GDT required. Any dimension that necessitated any tolerance other than the basic, has it's own tolerance listed. Other than that, the basic tolerance will be fine.

By: Kevin Andrews  Fri, 13 Oct 2017 20:37:52 GMT
Re: Geometric Tolerance - a second opinion

I'm haven't read through this whole thread. You wouldn't use parallel on an axis like that. Think about how would you inspect this part?

 

The slot needs a radius call-out FULL R .34 or something. You may use a diametric (but is not common for slot ends).

 

That's a true position call-out you should use. If you need the axis to be within/out .015 either way. All dimensions to the slot are to be basic.

This means that you can have .015 plus or minus sheet tol for 9.63 (which is to be theoretically perfect) in either direction.

 

It would be best if you had a secondary datum. Using the NPT Axis as your secondary (DATUM B), and the flat face of the NPT opening as Primary  datum A.

You need a dimension from the flat of the NPT.

 

You could also use profile of a surface to get the same result.

 

sorry for the horrible doodle.

By: Scott Casale  Fri, 13 Oct 2017 20:42:49 GMT
You are not authorized to view this page No results found! Suggestions: Check spelling, try a different search, or browse topics below.