Fit Callouts for Dowel Holes

[toph8674]

Hey Guys,

I'm trying to standardize the way I callout my dowel holes. I typically use oversized dowels from McMaster-Carr with m6 fits.
I typically use H7 fits because it is common and seems to give a good locational fit or sometimes a light mallet tap. But I have also used F8 and G7 for more clearance and K7 for a press fit.
I typically call them out like so...

5.012
5.000 H7 X 7.0mm DEEP

My questions are 1) Are there certain fits that you would prefer/not prefer because you typically stock the reamers or does it not make any difference to you?
2) Is there a way that you like to see dowel holes called out? I have also seen callouts like (5mm DIA X 7.0mm DEEP, REAM TO CLEARANCE FIT FOR 5m6 DOWEL).
I prefer the first way because I assume it is less work for the machinist and a bit more defined.

 

[Mtndew]

Is there a way that you like to see dowel holes called out?

I prefer the easy way:
PF for 10mm dowel x 20mm deep
SF for 10mm dowel x 20mm deep

 

[in2glamisgirl]

1. The greater the tolerance the better. The benefits of a wider tolerance band equals wider manufacturing options and lower scrap rate.

2. In Aerospace work I have never seen class of fit callouts, always a size and tolerance.
I.E. Ø 5.05-5.15mm x 20mm deep or Ø5.05mm +.10/-.00 x 20mm deep. Some machinists are not familiar with class of fit charts, just one more chance to make a mistake.

 

[implmex]

Hi toph8674:
Many many ways to call out dowel fits and shaft fits.
All of them are a pain in the ass for the machinist.
There are tables to consult in Machinery's Handbook, and judgments to make and symbol interpretations to make.
All this makes for loads of room for errors...not because they're ambiguous, but because they are so damned cumbersome to use and to interpret.
Specifying an "RC-1 fit" on a 1 mm dowel means you have to find out what the limits are for this size dowel, then you need to know the limits that are called out for this class of fit (clearance in this case).

Thankfully there are calculating tools available on the internet to help you like this one:

Preferred Tolerances Inch Units Chart ANSI B4.1 Calculator RC - LT Fits

This Calculator will determine the preferred size and limit tolerances for Running or sliding to interference-locational fits per ANSI B 4.1.

www.engineersedge.com

So it's not as bad as it used to be but it's still stupidly complicated.


When I'm in a dickish mood, I like to assign blame for this on lazy-ass engineers who can't be bothered to figure it out themselves but want to shift the effort onto us poor machinists.
When I'm feeling more charitable, I can see why the standard is there and that it has benefits as well as shortcomings.

I'm with Mtndew on this, but I'll go it one better:
Instead of "PF" or "SF" on the drawing I will write "Press Fit" and "Slip Fit" on the drawing so I don't get a phone call asking...What does "PF" mean??

Yeah it doesn't define the limit specifically, but who the hell can interrogate a reamed dowel hole to the requirement of the standard anyway, and who would take the time and the trouble for the vast majority of dowel holes.
Add to that the fact that dowel pins you can buy from McMaster are neither very round, nor are they very straight, and it becomes quickly apparent that you have to control a lot more than just what reamer to stuff in the hole if you want to work to the fits the standard expresses.

That's my rant for today.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[guythatbrews]

I'm of the explicit tolerance school of thought rather than class of fit tolerancing.

A lot of the european drawings I've seen use class of fit tolerance and I expect where the parts are being made might have an influence on which method to use. In Merica class of fit seems not as popular and it seems to me a waste of time, and a source of error. Everyone that touches the drawing has to look up the limits rather than the one time it takes to explicitly call out on the drawing. In short, it's a PITA.

I can't speak to the actual tolerance band for each size, but "sf" and "pf" may be common in some industries and considered shaky in others.

 

[toph8674]

Thanks for the responses,
The machinery's handbook gives incredibly tight tolerances for fits and many times dowels (particularly plastic) have a tolerance of ±0.005" which practically makes hitting the hole tolerance irrelevant anyway.
It sounds like there is reasonable consensus that you would prefer we callout press fit or a slip fit.
So in reality if I callout 5mm press fit or 5mm slip fit what do you try and target?
Press Fit: 4.95mm±0.05? Slip fit 5.05mm±0.05?

 

[dandrummerman21]

Well I think in inches, and for a 5mm hole I'd probably try for a .0005 press fit for steel, or up to a .001 for aluminum. That's about .012-.025 press. you wouldn't want 4.9 for a 5mm dowel unless you're doing plastic (no experience here).

So if you're doing plastic, and you want up to a .1mm press fit, you better specify it. Because you wouldn't get it from me unless you asked.

Basically, I'd get a 5mm gage pin and try to stick it in the hole. For a press it better not start. And for a slip fit it better not hang up but better not be sloppy either.

 

[toph8674]

Okay, I think thats good enough for what I need. Thanks guys!

 

[plastikdreams]

Press fit or slip fit...one is a thou under one is half a thou over...done.

 

[implmex]

Hi again Guys:
There is a caveat:
It depends on the size of the dowel.
Try to leave a thou for press fitting a 1 mm dowel and you'll probably fold it in half in the press.
Certainly for the teeny stuff I make, you'll bend the snot out of the part you're pressing the dowel into.

Similarly if you build big shit with big dowels... a one thou press on a one inch dowel isn't enough to hold squat.

But if a 1/4" dowel is your most common size then yeah...one thou of press is pretty good.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[SeymourDumore]

About the class of fit designations, I am fully in the camp of who say those should stay in the engineering room and never ever be put on the print!
If the engineer doesn't know the class of fit designation and the values, he/she can look it up and put it on the print explicitly.
If the engineer does know the designation and the values, he/she can pat him/herself on the back and then put it on the print explicitly.
In any case, put the friggin' tolerance band on the print explicitly!!!

 

[plastikdreams]

Hi again Guys:
There is a caveat:
It depends on the size of the dowel.
Try to leave a thou for press fitting a 1 mm dowel and you'll probably fold it in half in the press.
Certainly for the teeny stuff I make, you'll bend the snot out of the part you're pressing the dowel into.

Similarly if you build big shit with big dowels... a one thou press on a one inch dowel isn't enough to hold squat.

But if a 1/4" dowel is your most common size then yeah...one thou of press is pretty good.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

I dunno Marcus, I've used the 1k formula with .750 pins and it worked just fine...that was a US .001 not a Canadian .001

 

[Nmbmxer]

I knew a guy that reamed every dowel hole to the same size (+.0005), if it was called out as a "press fit" he shrunk the top with a ball bearing. This was for onesie twosie parts in a toolroom.

I personally like performance based metrics rather than generic fit tables, though there is a time and place for controlling everything vs the understanding that the dowel can't fall out during assembly, the trick is learning when being a little sloppy is acceptable. Generally when you make and assemble the thing there is more leeway than when you purchase the bits and want to blame someone when it doesn't work 100.00000% of the time.

 

[implmex]

Hi again plastikdreams:
If I use the calculator I linked to, but put in a force fit designation (FN5) it spits out an interference allowance of up to 0.0033" for a 1" dowel.

That's what the "Bible" says... not to insist it's the only way, but it is what ANSI specifies, so if it's on a drawing, it's what they intend you to follow, and if it's not on the drawing you may well find that it works just fine to allow 0.001"
.
As an aside, I built injection molds for a living for decades, and we too allowed 0.001" press fit for leader pins and had no issues...in fact, the shanks on 3/4" pins are 0.751" diameter and are intended to be pressed into a reamed 0.750" diameter hole.

So you make a very good point about the difference between an engineering fantasy and a machinist's practical reality (Canadian OR American ).
It also made the tone of my remark in post #10 sound like it's "all wrong" to do what you advocated...that was clearly Bullshit and I apologize.
I should have made clear that this is what ANSI specifies for press fits...not what actually works and is used in the real world.

But you still cannot leave 0.001" press fit for a 1 mm dowel...it's more like 0.0001" to 0.0002" if you want to have a hope of getting it in without bending it or bending the part it's supposed to go into.
I routinely ream nominal and just polish down and Loctite the little fuckers in...saves a lot of pain but it sure violates the "rules".
Good thing I'm mostly Alpha prototyping and get to use my own judgement.

For the vast majority of dowels we do not need to be so ridiculously anal, and going back to the OP's question, if you put it on the picture it becomes Gospel, whether it's a good idea or not.

Safer to just specify Press Fit, Push Fit or Slip Fit even if it's not the "Correct ANSI Way".
Any competent machinist will know what to do.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Mtndew]

I've also seen for a slip fit callout:
slip fit no shake or SFNS.

 

[plastikdreams]

Hi again plastikdreams:
If I use the calculator I linked to, but put in a force fit designation (FN5) it spits out an interference allowance of up to 0.0033" for a 1" dowel.

That's what the "Bible" says... not to insist it's the only way, but it is what ANSI specifies, so if it's on a drawing, it's what they intend you to follow, and if it's not on the drawing you may well find that it works just fine to allow 0.001"
.
As an aside, I built injection molds for a living for decades, and we too allowed 0.001" press fit for leader pins and had no issues...in fact, the shanks on 3/4" pins are 0.751" diameter and are intended to be pressed into a reamed 0.750" diameter hole.

So you make a very good point about the difference between an engineering fantasy and a machinist's practical reality (Canadian OR American ).
It also made the tone of my remark in post #10 sound like it's "all wrong" to do what you advocated...that was clearly Bullshit and I apologize.
I should have made clear that this is what ANSI specifies for press fits...not what actually works and is used in the real world.

But you still cannot leave 0.001" press fit for a 1 mm dowel...it's more like 0.0001" to 0.0002" if you want to have a hope of getting it in without bending it or bending the part it's supposed to go into.
I routinely ream nominal and just polish down and Loctite the little fuckers in...saves a lot of pain but it sure violates the "rules".
Good thing I'm mostly Alpha prototyping and get to use my own judgement.

For the vast majority of dowels we do not need to be so ridiculously anal, and going back to the OP's question, if you put it on the picture it becomes Gospel, whether it's a good idea or not.

Safer to just specify Press Fit, Push Fit or Slip Fit even if it's not the "Correct ANSI Way".
Any competent machinist will know what to do.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

I thought your post was fine. Smallest I deal with is .0625 lol...you and your tiny crap

 

[triumph406]

If you don't achieve the desired ppess fit on the dowel, there's always loctite.

I should probably provide free loctite to my customers, I've had a few press fit holes be slip fit over the years. Haven't lost a lot of sleep over the problem when loctite can be used

 

[Ox]

I know it's been said a cpl'a times already, but I have gotten too many prints through here with those H this and g that.
BOY - what a time suck!

I'm not even above having the charts taped up on the wall, but doo you have any idea how many pages there is of those things?

The fit chart is handy for design porpoises - I git it.
But YOU look it up ONCE and put it on the print, and the rest of us won't have to time and aggin.




------------------

Think Snow Eh!
Ox

 

[SeymourDumore]

But YOU look it up ONCE and put it on the print, and the rest of us won't have to time and aggin.




------------------

Think Snow Eh!
Ox

'Zactly!

Wonder if there is anyone here on PM willing to defend the practice of indicating only the fit class over specifying the actual dimensions with numbers?

 

[Clive603]

'Zactly!

Wonder if there is anyone here on PM willing to defend the practice of indicating only the fit class over specifying the actual dimensions with numbers?

Horses for courses.

As has been said earlier class for engineering (and design) numbers for the machinist. Engineering design is ultimately about function. Calling out H7 immediately defines what the hole is for. Numbers need translation and reference to the mating part.

But if you are Mighty Big Industries Inc on serious production runs where significant quantities of bespoke tooling is called out and set out for long run jobs fit class callouts make sense on the print. Calling tooling is, fundamentally, a storekeepers function and at that end of the world its a darn sight easier to call out a reamer for a H7 fit rather than trust a non-specialist to figure out the undersize relative to nominal needed. For smaller outfits doing smaller quantities with the machinist multi-tasking numbers are the only way to go because you have to use what you have or can afford to get just one of for that one job.

Same on inspection to print. Mighty Big Industries Inc are set up to recognise the H7 hole and the CMM spits out go / no-go. Littler guy using pin gauges wants numbers.

Dills are different. Always numbers because it's assumed you have them all!

Me, on my own doing mostly "how the F... dit they mange to break that" and "come up with something that sort of does this, real cheap" stuff I'd love to just call out tooling to give the right fit. But it ain't gonna happen. Numbers all the way down. Imperial'n metric mix'n match is often the only way on "needs a miracle" repair stuff too.

Clive