Hello Guest it is September 24, 2023, 06:12:15 AM

### Author Topic: Turning a Morse taper  (Read 12047 times)

0 Members and 1 Guest are viewing this topic.

#### Segrest

• 24
##### Turning a Morse taper
« on: March 08, 2008, 10:11:18 PM »
Hello Everyone,

Now that I seem to have gotten through some of the basics, I though I would try turning a taper.

What I want to do is turn a Morse #2 taper on the end of a piece of round stock.

I pulled up my handy machinists reference and it tells me that the rate of taper for Morse #2 is 0.59941 inches per foot.  My handy dandy trig table tells me that the angle for the taper is equal to arc tangent of the rate of taper divided by the length (Arc Tan 0.59941/12) for 2.8596 degrees.

I started up the Mach3 Turn OD Taper Wizard and entered the following parameters:

X End:       0.5
Angle:       2.8596
X Start:     0.8
Z End:       2.3
Z Start:     0.0
Clearance:  0.1

I started the program and it ran without a hitch.

But, my pretty new taper doesn't fit...

I figure that I did something silly, can someone tell me what?

Bob

#### docltf

• 354
##### Re: Turning a Morse taper
« Reply #1 on: March 09, 2008, 12:37:07 AM »
segrest

did you figure half of the .59941
mt2   angle is 1deg   25min  50sec  or .2997 per foot
go get em.

bill

#### jimpinder

• 1,232
• Wakefield, West Yorks, UK
##### Re: Turning a Morse taper
« Reply #2 on: March 09, 2008, 04:12:50 AM »
Please don't misunderstand this post - I am a great believer in working things out for myself, and seeing what I think is the nub of the problem. The wizards are very good, and I use them myself, but - when things go wrong it leaves you high and dry trying to guess the problem.

Why are you bothering with the handy dandy trig table and the Wizard - you have the figures in front of you.

For every foot the taper is 0.59941 so the GCode is  (from 0,0) G1 Z12 X-0.59941.

You cannot do a straight cut - you will have to do some roughing cuts - but it is as simple as that.

If you are doing anything short of 1 foot - say 3,4 or 6 inches, divide the amount of taper by 4,3 or 2.

I haven't checked whether the taper applies to diameter or radius, as Bill said - but you can just alter the lathe from radius mode to diameter mode - wthout altering the maths.

Now if you did that and it didn't fit we can find out why, but unless I take the wizard apart line by line, I don't know.

I'm sure Bill has the answer, and I am sure your second go will work, but try writing simple GCode, it is quite rewarding.

« Last Edit: March 09, 2008, 04:33:25 AM by jimpinder »
Not me driving the engine - I'm better looking.

#### Segrest

• 24
##### Re: Turning a Morse taper
« Reply #3 on: March 09, 2008, 07:47:45 AM »
Hello Bill, Jumpinder,

I think Bill is on the right track.  I suspected a NUG error and am glad it is something simple.

Jumpinder's point is sound as well.  Manually coding the final pass is simple enough.  The wizard makes calculating the roughing cuts easy and but I recognize that I can write more efficient code myself.

Thank you both for your responses.  I will give it another whirl later today.

Bob

#### M250cnc

• 591
##### Re: Turning a Morse taper
« Reply #4 on: March 10, 2008, 08:39:21 PM »
Hi Bob

Another simple test is mount the morse taper you want to produce (Reamer Etc) in the lathe chuck between centres and  to substitute a DTI for the toolbit and check any error with the motor off.

When the toolpath exactly follows the morse tape with the DTI and it still doesn't come out right you will then know that you have mechanical issues.

Strictly speaking the finish should be ground.

HTH
Phil_H
The Good Thing About Mach3, Is It's very Configurable