Tapping Feedrate Precision Question

[Mike@Apollo]

Currently all linear feeds are posted with one decimal place precision. This isn't a problem for most operations, but operators are more comfortable seeing for places for tapping operations.

 

How/where would I change this to post four decimal place feeds for tapping ops?

 

Thanks.

[mtnflyr]

I'm not sure if this setting also affects tapping, but look into Systen Configuration - Analyze - Precision for Analyze Distance setting. The determines how far dimensions are carried after the decimal point.

[Mike@Apollo]

No, that doesn't affect the posted code at all.

 

I'm thinking somewhere either in the control def, or in the post itself. I just can't find it.

[iowajim62]

Look for this in your post in General Output Settings

code:

---

 tap_feed    : 1      #0 = 2/1 (in/mm) decimal places, 1 = 4/3 (in/mm) decimal places 

---

HTH

[Mike@Apollo]

I was able to find this:

code:

---

fs2 17  0.2 0.3      #Decimal, absolute, 2/3 place (tapping feedrate)  

---

Still doesn't explain one decimal.

[iowajim62]

Mike,

quote:

---

Still doesn't explain one decimal

---

No it won't you have to change what I showed earlier.

Your post has 0 change it to 1 and try it again.

[Tim Johnson]

What you grabbed is from the formats statements. You need to look in the format area;

 

code:

---

fmt  Q  2   peck1$       #First peck increment (positive)

fmt 2 peck2$ #Second or last peck (positive)

fmt 2 peckclr$ #Safety distance

fmt 2 retr$ #Retract height

fmt K 4 repeat #canned cycle repeating

fmt Q 2 shftdrl$ #Fine bore tool shift

fmt Z 2 entryz #Entry Z for custom drill

fmt Z 2 zdrl$ #Depth of drill point

fmt Z 2 tosz$ #Drilling top of stock

fmt N 4 n_tap_thds$ #Number of threads per inch (tpi) / Pitch (mm)

fmt F 13 pitch #Tap pitch (inches per thread) #<<<<<<<<<<<<<<<<<<<<

fmt R 2 refht_a #Reference height

fmt R 2 refht_i #Reference height

---

The marked line is what I use but you may use something else. Look for a tapping variable there and replace the number to 17.

[Guest CNC Apps Guy 1]

If I absolutely HAVE to tap, I ALWAYS tap in IPR and go to 3 decimal places. Fit has always been good so long as I did things right.

[Dave Ball]

Ditto that Apps Guy!

[MotorCityMinion]

Feed IPR for tapping may require a parameter change in the actual machine control.

[Mike@Apollo]

Thanks everyone for your input.

 

After some digging, I found this:

code:

---

 pcanceldc$       #Cancel canned drill cycle

result = newfs(12, feed) #WAS (9, FEED)<<<<<<<<<<<<<<<<<<<<<<<

result = newfs(three, zinc)

result = nwadrs(strq, peck1$)

z$ = initht$

if cuttype = one, prv_zia = initht$ + (rotdia$/two)

else, prv_zia = initht$

pxyzcout

!zabs, !zinc

prv_gcode$ = zero

pcan

pcan1, pbld, n$, sg80, strcantext, e$

pcan2

---

I changed the "(9, feed)" to "(12, feed)" and it seems to do what we want.

[Guest CNC Apps Guy 1]

quote:

---

...Feed IPR for tapping may require a parameter change in the actual machine control...

---

Generally it is a standard option included with the machine. I think in all my years running machines I've seen less than 10 that did not have it and all were late 80's machines or older.

 

JM2C

[Dave Ball]

Most of the time all you need to do is use G95 to switch to IPR and give the feed in IPR, then G94 to switch back to IPM when done tapping.

[Mike@Apollo]

CNC Apps Guy,

I would rather thread mill also, but this particular application requires a 3/8-24 thread over 4" deep. Without the four place feedrate, bad things happen unless the RPM's support a feedrate without a decimal.

 

How can IPM be switched to IPR in the post?

[Dave Ball]

Look for this switch in your post.

 

 

code:

---

use_pitch : 1 #0 = Use feed for tapping, 1 = Use pitch for tapping

---

[Dave Ball]

Actually...this is what is in my post.

 

code:

---

pmisc2$          #Canned Rigid Tapping Cycle

pdrlcommonb

#RH/LH based on spindle direction

pbld, n$, sg95, e$

pbld, n$, sm29, *speed, e$

if met_tool$, pitch = n_tap_thds$ #Tap pitch (mm per thread)

else, pitch = 1/n_tap_thds$ #Tap pitch (inches per thread)

pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *pitch, !feed, strcantext, e$

pcom_movea

---

[MotorCityMinion]

Quoting the Quote. -.-

 

quote:

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

...Feed IPR for tapping may require a parameter change in the actual machine control...

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

 

Generally it is a standard option included with the machine. I think in all my years running machines I've seen less than 10 that did not have it and all were late 80's machines or older.

_________________________________________________

If it's standard, then its not an option. Anyone want some Jumbo Shrimp?

[Guest CNC Apps Guy 1]

quote:

---

...If it's standard, then its not an option...

---

You must not be too familiar with how FANUC operates. EVERYTHING is an option. When they sell a control to a machine tool builder, they get HARDWARE ONLY. The builder then goes down the list and says, "...I need this, I need that, oh, and I guess we'll take the other thing as well..." etc...

 

There are generally speaking, standard sets of options.

 

HTH

[MotorCityMinion]

Actually, we have a 18i controller on a Makino S50 with very few options on it. It totally suxs. $250k of uselessness as our Haas machines are much more flexible and way easier to set-up and at 1/3 the cost. I started out on a 6m, then went on to Mazaks for quite a few years and have not seen much of the Fanuc's untill recently.

[Guest CNC Apps Guy 1]

I feel your pain. Kitamura HMC's come with an impressive list of Options (Extended Offsets, Dataserver, Ethernet, NURBS, Custom MACRO B, etc...) but still only come with Tool Offset "A"(H and D cannot match).

 

Toyoda HMC's (with 16i's) come with CUstom MACRO B, Tool Offset "C" (H, H Wear, D and D Wear), G54-G59 , and NO HELICAL Interpolation

 

You know darn well that a bean counter made the decision on what options would be standard.

 

:sigh:

 

Tell you what though, I'd take that Makino over a Haas any day of the week. It's a FAR superior machine tool even with the control being stripped down.

[Dave Ball]

quote:

---

Tell you what though, I'd take that Makino over a Haas any day of the week. It's a FAR superior machine tool even with the control being stripped down.

---

+1 to that Apps Guy