tap feed is wrong...

[bbtom]

When tapping in mastercam I put 100 in the spindle speed and I click in the feed area and mastercam gives me the proper feed for that tap and spindle speed.

 

The problem is the decimal point in in the wrong spot.

 

Say I have a 4-40 tap.

I want to run 100 spindle speed. I take the number 1 and divide by the pitch 40.The answer is .025 this is what I want in the feed area when I click in the box.

 

BUT what I get when I click in the feed box is 2.5

 

how can I fix this???

 

Thank You

[J Coulston]

MasterCam displays IPM. You are looking for IPR, both are correct. I will depend on your post as to what is output.

 

G95 IPR F.025 Preferred method for tapping

G94 IPM F2.5

 

If you are running X4 the parameter tool tab will show both IPM and IPR. Feed Rate and FPT.

[J Coulston]

Here is an example.

 

N767 G90

N768 M29 S1500

N769 G95 <-----

N770 G98 G84 Z-.05 R.33 F.025

 

 

N767 G90

N768 M29 S1500

N769 G94 <-----

N770 G98 G84 Z-.05 R.33 F2.5

[heavychevy2155]

How are getting it to post a G98, I can only get G99 to post for some reason? This is with X4 MPMASTER.

[J Coulston]

I hard coded it, G99 burnt me once, so I fixed it to always retract.

 

sg99 : "G98" #Reference at refht

[Colin Gilchrist]

There is probably a switch at the beginning of your post: use_pitch

 

If you set this variable to "1" you should get pitch output. This will also change the behavior of the "feed rate" parameter to properly show you "0.025" when you change the spindle speed to "100".

 

Is there any particular reason you are tapping so slow? What material and type of machine? The reason I ask is that I tap at between 250 and 1000 RPM in aluminum...

 

HTH,

[bbtom]

I didn't realize 100 rpm was that slow.

 

I use that tap feed for everything from aluminum to tool steel.

 

I will look for the switch... use_pitch

 

 

Thank you

 

...also, I am using X3....

[Colin Gilchrist]

It really depends on your machine though. 100 RPM might be ok if your machine doesn't do well at higher speed/feeds.

 

What machine? What control? How old?

 

On a Haas machine you can also set a parameter to increase the speed while retracting out of a hole. I can tap in at 500 rpm and reverse out of the hole at 4x that speed (2000). Makes for some quick holes...

[bbtom]

machine is deawoo, fanuc series 21imb controller, i think bout 5 years old

[Thad]

quote:

---

On a Haas machine you can also set a parameter to increase the speed while retracting out of a hole.

---

My beloved Fadals can do the same thing.

 

 

I guess it's a coincidence that the IPR feed and IPM feed make it look like it's a decimal point error, rather than a feed type error. There probably aren't too many feed rates that will look like that.

 

Thad

[Colin Gilchrist]

You should be able to tap aluminum at 500-1000 RPM on that machine.

 

This does assume you have a rigid holder. I wouldn't do that in a a drill chuck.

 

You can tap at any speed that you are comfortable with. If you have a lot of holes to do then I'd recommend you speed it up a little bit.

 

Also, can you form/roll tap these parts? I find I can go about 30% faster when form tapping vs. cut tapping.

[frostfritt]

I have a warning here..

Lets say you have a pitch output and MC X4 and want to change the pitch just for once in your tapoperation. It can be done and the new value stick and look fine but the post takes the rpm from the operation and the pitch from the tool.

 

If you post and run that nc file, then the tap and part will go to the blue archive

 

You have to always do a new taptool first.

 

/frostfritt