What's new
What's new

Make a 16/32 T15 spline correcly to wedm

panscan

Plastic
Joined
Aug 20, 2016
Hi,

I have been looking at Involute Spline ANSI B92.1 Involute Spline ANSI B92.1 Equations and Design | Engineers Edge | www.engineersedge.com

I need to make a drawing to edm a internal spline 15T 16/32 ansi flatroot side fit spline. normal tolerance.


How do I know the clearande for internal and external without having a measurment between pins. I can only find on the bottom of that page "0.001D" does that mean 0.001in of contour clearance or 0.001 x 16 = 0,016? or 0.001in in contour clearance? Is there a was to add this clearance to the spline or do I have to make it nominal and then compensate the tolerance when machining? Or would change the measurment betweenn pins in mastercam by the amount of clearance I want do the trick? Which way is the most correct one todo?


I attach the settings i have in mastercam right now.

Any input would be good. Thanks


Here is the original thread with the attached picture of my settings.

CAD a 16/32 t15 spline correcly, any splines guys here ?
 
Hi panscan:
I can't speak to the tolerance requirements of the spline but I can offer some recommendations on how to determine if you got there, especially on an internal spline.
As you know, the wire will cut very accurately and very repeatably, so with stuff like this that I need to get dead nuts but can't measure easily I do a simple circular cut first in the waste stock at the center of the bore.
I rough it, I skim it and then I measure it and see what I got.

If my settings are good, I cut my final part shape and trust the machine to do it all again accurately.

If my settings are not good, I change them BUT I CHANGE ALL OF THEM.
My roughing pass, my semifinishing pass, and my skim pass all get changed by the same amount to compensate for the difference between what I got and what I tried to get.
If it's super critical I make a new set of passes at a new diameter and measure the result again.

When all is good I commit and cut my final shape.

With regard to your question about how to best create the clearance, be aware that just comping the wire gives you a different outcome from following the proper profile with the clearance already incorporated, that's especially noticeable in the corners.
Comping out the wire gives you progressively smaller external corners and progressively bigger internal corners. (it fucks up everything else too but on an involute profile it's hard to tell)

Following the commanded path even with nominal comp invoked gives you exactly what the CAD file requires.

Moving on to the calculation, it seems to me that your link describes the clearance as 0.001 multiplied by the pitch diameter "D" (so 0.001 x D) to a maximum of 0.010" and a minimum of .002"
So for a pitch diameter of 10" the clearance would be 0.010" and for every diameter bigger than that it would also be 0.010"
For a 2" pitch diameter it would be 0.002" and it would still be 0.002" for any size smaller than 2" diameter.
Between those sizes the formula applies.
That is the RADIAL form clearance:
Here's a snip from the formula chart referenced in the linkspline chart.JPG


Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Hi,


I'm using mastercam gear hook to make the spline drawing. 15 teeth and the pitch diameter are 23.8125mm so 0.002 clearance then. But how do I add it to the contour correcly.

15 teeth
16/32 dp ansi flatroot side fit spline.

taking spline info from Involute Spline ANSI B92.1 Equations and Design | Engineers Edge | www.engineersedge.com



Can verify this:

Pitch Diameter "D" = 15/16 = 0,9375in x 25.4 = 23,8125mm
Major Diameter Internal "Dri" = (N + 1.35) / P = 15 + 1.35 / 16 = 1,021875in x 25.4 = 25,9556mm
Minor Diameter Internal "Di" = (N - 1) / P = 15-1 / 16 = 0.875in x 25.4 = 22,225mm

And the last two:

Form Diameter, Internal = (N + 1) / P + 2cF
Form Clearance (radial) cF = 0,001D, with max of 0.010, min of 0.002

I attach the gear hook printscreet from mastercam. How do I correcly add this tolerance to the whole form/contour? Add this value to the measurment over pins feels like it only open up the flank clearance?

How would you do it?

Its not a high tolerance spline I just want to understand how to make it and add the tolerance :) Thanks
 

Attachments

  • spline.jpg
    spline.jpg
    87.1 KB · Views: 71
Hi panscan:
Make the profile of the nominal male spline in Mastercam using the Gearhook utility you're accustomed to using, with the values for the male spline.
Then do an offset contour in Mastercam with your clearance amount as the offset.
Make sure it offsets in the correct direction.
Program your female spline using the offset contour.
You're done!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Hi,

Thanks, thats actually smart. But... will that really be correct? It feels like the Minor and major dimentions are going to be too small if I do it like that.

Why not making it as a internal spline in the gearhook and then offset it with 0.002in ? then the major are dimentions have more clearance. Major Diameter Internal "Dri" = (N + 1.35) / P = 15 + 1.35 / 16 = 1,021875in x 25.4 = 25,9556mm otherwise im affraid the fillets/radius on the tip of the spline will be too shallow if the male part (that I dont machine or have seen) dont have any radius on the corners.

would it not be correct to do it that way?
 
I did a test, make one internal and one external spline in mastercam gearhook. And this is the result (see picture).

From this I think the most accurate way would be to make the spline as a internal but with Major and minor minus "(the given tolerace that you are going to offset the contur with)" to get the correct form. Becouse the major and minor is static and not tolerance based measurments right?


Can anyone verify if I'm right? thanks
 

Attachments

  • spline2.jpg
    spline2.jpg
    46.5 KB · Views: 46
Customer job, I dont have the male part. I just need to make sure my internal will fit correcly :)
 
Customer job, I dont have the male part. I just need to make sure my internal will fit correcly :)
Flat root and full fillet will both fit the mating part fine, so if they give you a choice and you have the wall thickness, then fillet root is better.

More so on the male, but still worth it on the female if you can. Shaping can be kind of a bitch because of the extra depth of the cutter but you're going to edm it, yes ?

By the time you're done, you may find it was easier to sub it to a guy with a Fellows :)
 
Good morning All:
Sadly I lied to you all in post #4.
The specification referenced by the OP clearly states that the FEMALE spline is nominal and the male spline is adjusted to suit.
I got it exactly backward.

This makes sense when you consider that before wire EDM, the way to make spline pairs was to broach the female (or cut it on a Fellows shaper) and hob the male (or shape it too).
A big pull broach is an expensive piece of kit, so it is reasonable that those would be made nominal, so a spline manufacturer would only need to stock one for any size.

The "easier" part to adjust would have been the male spline, so depending on the precision required of the pair, the clearance would be put on the male.

Fast forward to the modern era:
We have wire EDM, so making a female spline is easy and making it any size we want is easy.
What I don't know is whether the standard has shifted to accommodate the new reality.
I suspect not.

So if that's the case, the female spline has to be cut to nominal: whether with a broach, a shaper, or a wire EDM doesn't matter.
Theoretically, if I'm not full of it, the female profile is made nominal in CAM, and is cut to nominal on the wire.
The male will already have the proper clearance for the tolerance class of the spline pair and will fit into a nominal female.

So, all spline experts (I'm obviously not one of them) is my reading of the OP's original specification correct or not??

Cheers

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

Attachments

  • female spline spec.JPG
    female spline spec.JPG
    59.8 KB · Views: 29
A big pull broach is an expensive piece of kit, so it is reasonable that those would be made nominal, so a spline manufacturer would only need to stock one for any size.

The "easier" part to adjust would have been the male spline, so depending on the precision required of the pair, the clearance would be put on the male.
That sure makes logical sense. But doesn't the standard linked in post #1 say the opposite?
Last time I talked to Ash about a broach, they told me SAE spline broaches came in several sizes and you bought the broach needed to create the the fit you wanted.
I'd like to know the answer too.
 
Hi Mud:
Here's the part of the spec that I interpreted the way I did:
"The internal spline is held to basic dimensions and the external spline is varied to control the fit"

I read that to mean the female spline is made nominal.
What part of the standard are you seeing that you interpret the opposite?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

I read internal to mean the male (inside)part and external to mean the female (outside) part. I've confused myself. Again.

But then why did Ash offer me a choice of broaches for different fits?
 
We have wire EDM, so making a female spline is easy and making it any size we want is easy.
What I don't know is whether the standard has shifted to accommodate the new reality.
New reality is the same as the old reality - a broach pulls a spline in less than thirty seconds. It will be a while before wire edm can touch that :)

No the spec confused us both and now nobody will ever know!
Scholars will have scholarly arguments and hate each other for a thousand lifetimes.
Splines are a mess. I think the splines came first, then they tried to create standards to fit. But there was no standardization in what people had already done, so that was a futile effort. They are all different.

Metric module involute splines are a great example. Thirty years ago or so there weren't any - even metric cars had inch splines. So then they created metric splines, but all those were was inch splines with translated dimensions. Them yuropeens finally created fully metric splines, but now you had competing metric splines and all fit some standard or other, but not the same one ....

The situation is (imo) better with straight-sided splines, but mostly because people didn't use involute splines as much in the past. They weren't as common, so you didn't have as many different implementations. Ime, if it's something new and you're making both parts or have prints, making it "to the standard" will be okay but if it's a repair or replacement part, better measure a sample, chances are real good the parts preceded the "standards". Or whoever made it just ignored them. There's no penalties :)

Not much in automotive is "standard" anyhow, when you make two million of something you can set your own standards, and they do.
 
thanks for venting the ideas!

but back on topic again..

still one question, if the internal splines are nominal, why does the Form Diameter and Major Diameter Internal "Dri" talks against each other?

  • Major Diameter Internal "Dri" = (N + 1.35) / P = 15 + 1.35 / 16 = 1,021875in x 25.4 = 25,9556mm
  • Form Diameter, Internal = (N + 1) / P + 2cF = 15 + 1 / 16 + 0.01 = 0.999in = 25,3841mm

Why is there a form clearance is its nominal. Acording to this doc Involute Spline ANSI B92.1 Equations and Design | Engineers Edge | www.engineersedge.com
the form clearance is the minor/major clearance between internal and external tips?




Can verify this:

Pitch Diameter "D" = 15/16 = 0,9375in x 25.4 = 23,8125mm
Major Diameter Internal "Dri" = (N + 1.35) / P = 15 + 1.35 / 16 = 1,021875in x 25.4 = 25,9556mm
Minor Diameter Internal "Di" = (N - 1) / P = 15-1 / 16 = 0.875in x 25.4 = 22,225mm

And the last two:

Form Diameter, Internal = (N + 1) / P + 2cF
Form Clearance (radial) cF = 0,001D, with max of 0.010, min of 0.002
 








 
Back
Top