Tapping Head setup

Yahoo posts
1

I am trying to setup my mill to use a Stm JSN7 tapping head. It self feeds for 0.14" after the feed stops, then goes into neutral. I set up the tool using Axial Travel at 0.14" this is the Gcode generated. for a hole tapped to 0.500" deep


N0010 (Filename: Taig CNC Lead Screw Nut.tap)
N0020 (Post processor: Mach3.scpost)
N0030 (Date:30/05/2014 Time:12:17:02)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: Taig CNC Lead Screw Nut)
N0080 (Operation: Tap, 10-32_THREADS, T12: Tapping head #10-28 tap, 0.5 in Deep)
N0090 S500 G00 Z3.0000
N0100 X0.0000 Y0.0000
N0110 (Tapping head #10-28 tap)
N0120 T12 M06
N0130 G43 H12
N0140 G00 Z0.1250
N0150 S1000 M03
N0160 M49
N0170 G95
N0180 X-0.4970 Y-0.7263
N0190 Z0.0394
N0200 G01 Z-0.500 F0.0357
N0210 Z-0.360 F393.7008
N0220 Z0.179 F0.0714
N0230 G00 Z0.1250
N0240 X-1.1220 Y-0.5388
N0250 Z0.0394
N0260 G01 Z-0.500 F0.0357
N0270 Z-0.360 F393.7008
N0280 Z0.179 F0.0714
N0290 G00 Z0.1250


Then on to the next hole.



On line 200, it gives the feed down to z -0.500, then on line 210 tries to jump back to z -0.360 at an extreme feed rate then on line 220retract at the 2x retract speed to Z 0.179. Where does the z0.179 come from?



It would seem that feeding to z-0.360 and then a pause of four index pluses then the 2x retract would be a better method. I worry that the quick jerk back from depth might stall my z axis stepper and if this were to happen, the tap would continue to self feed.to z -0.614"


This is my first attempt to CNC feed the tapping head.and I want to understand what is going on before commenting a tap to metal.



Don

.,._
Posted by: Don@Campbell-Gemstones.com

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

2
<?xml version="1.0"?>
3

Hi Brian,


I gave up on using the tapping portion of Sheetcam because I kept getting odd rapids on the way out and things just didn’t make sense.

Could you describe your ideal sequence of moves for tapping. I don’t have a tapping head here so I’ve never tested the moves myself.

Les


.,._
Posted by: Les Newell <les.newell@fastmail.co.uk>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

4

Hi Les,

Sure, but there are several styles of tapping, so I’ll describe what I do in each case. Now, I don’t have rigid tapping so that won’t be a method I know about.


First, this is how I do tapping with “Tension and Compression” style holders, this is where you have to reverse the spindle. The advantage to this style holder is I don’t have to have a torque arm on my mill, which is rather difficult to set up on a moving quill knee mill.


N2010 (1/4-28 tap)
N2020 T6 M06 G43 H6
N2030 M07
N2040 S1000 M03
N2050 G00 X.19 Y-2.75
N2060 Z-1 (my hole surface is down at Z-1.3)
N2070 G01 Z-1.8 F35.7 (feed is 1/28 time the rpm)
N2080 M04 (Reverse the spindle)
N2090 G04 F1 (Dwell for one second, my spindle takes that long to stop and reverse, this varies with rpm)
N2100 Z-1 (feed back out)
N2110 M03 (back to forwards speed)
N2120 G00 Y-.25 (on to next hole and repeat)
N2130 G01 Z-1.8
N2140 M04
N2150 G04 F1
N2160 Z-1
N2170 M03
N2180 G32 (retract to tool change position)



Now, if I use my Tapmatic it goes a little different, I have an NC-1 which reverses at the same speed as forwards. A lot of Tapmatics reverse at 1.5 or 1.75 times the forward speed so increased feedrate would need to be set up.


(1/4-28 tap)
T6 M06 G43 H6
M07
S1000 M03
G00 X.19 Y-2.75
Z-1
G01 Z-1.8 F35.7
G04 F.1 (short 1/10 second dwell to allow the pullout and release)
Z-1
G00 Y-.25
G01 Z-1.8
G04 F.1
Z-1
G32



I don’t go to the trouble to use the tapmatic unless I have like 5 or more holes per part, and I can load the head into the spindle, engage the torque arm and just leave it in the spindle and change the parts in the vise and just do the tapping cycle as a separate operation on my parts. If you have a toolchanger, then you are talking a VMC and they have brackets and such to act as torque arms and will work through a toolchange.


In both cases, I’m allowing for pull out, or over run myself, like I said before, so darn many variables, that’s it’s just easier to program way shallow and then adjust the code and be done with it.


I hope that helps…. let me know if you have any other questions.

Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 2, 2014, at 3:50 AM, Les Newell les.newell@fastmail.co.uk (les.newell@fastmail.co.uk) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Hi Brian,

I gave up on using the tapping portion of Sheetcam because I kept getting odd rapids on the way out and things just didn’t make sense.

Could you describe your ideal sequence of moves for tapping. I don’t have a tapping head here so I’ve never tested the moves myself.Les
\



.,._
Posted by: Brian Lamb <blamb11@cox.net>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

5

Thanks Brian,

I think the main thing missing from SheetCam’s Tapmatic tapping code is the dwell at the bottom.

Les

On 02/06/2014 14:36, Brian Lamb blamb11@cox.net (blamb11@cox.net) [sheetcam] wrote:

Hi Les,

Sure, but there are several styles of tapping, so I’ll describe what I do in each case. Now, I don’t have rigid tapping so that won’t be a method I know about.


First, this is how I do tapping with “Tension and Compression” style holders, this is where you have to reverse the spindle. The advantage to this style holder is I don’t have to have a torque arm on my mill, which is rather difficult to set up on a moving quill knee mill.


N2010 (1/4-28 tap)
N2020 T6 M06 G43 H6
N2030 M07
N2040 S1000 M03
N2050 G00 X.19 Y-2.75
N2060 Z-1 (my hole surface is down at Z-1.3)
N2070 G01 Z-1.8 F35.7 (feed is 1/28 time the rpm)
N2080 M04 (Reverse the spindle)
N2090 G04 F1 (Dwell for one second, my spindle takes that long to stop and reverse, this varies with rpm)
N2100 Z-1 (feed back out)
N2110 M03 (back to forwards speed)
N2120 G00 Y-.25 (on to next hole and repeat)
N2130 G01 Z-1.8
N2140 M04
N2150 G04 F1
N2160 Z-1
N2170 M03
N2180 G32 (retract to tool change position)



Now, if I use my Tapmatic it goes a little different, I have an NC-1 which reverses at the same speed as forwards. A lot of Tapmatics reverse at 1.5 or 1.75 times the forward speed so increased feedrate would need to be set up.


(1/4-28 tap)
T6 M06 G43 H6
M07
S1000 M03
G00 X.19 Y-2.75
Z-1
G01 Z-1.8 F35.7
G04 F.1 (short 1/10 second dwell to allow the pullout and release)
Z-1
G00 Y-.25
G01 Z-1.8
G04 F.1
Z-1
G32



I don’t go to the trouble to use the tapmatic unless I have like 5 or more holes per part, and I can load the head into the spindle, engage the torque arm and just leave it in the spindle and change the parts in the vise and just do the tapping cycle as a separate operation on my parts. If you have a toolchanger, then you are talking a VMC and they have brackets and such to act as torque arms and will work through a toolchange.


In both cases, I’m allowing for pull out, or over run myself, like I said before, so darn many variables, that’s it’s just easier to program way shallow and then adjust the code and be done with it.


I hope that helps…. let me know if you have any other questions.

Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )



On Jun 2, 2014, at 3:50 AM, Les Newell > les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> ) [sheetcam] <> sheetcam@yahoogroups.com > (> sheetcam@yahoogroups.com> )> wrote:

Hi Brian,

I gave up on using the tapping portion of Sheetcam because I kept getting odd rapids on the way out and things just didn’t make sense.

Could you describe your ideal sequence of moves for tapping. I don’t have a tapping head here so I’ve never tested the moves myself. Les

\

\



.,._
Posted by: Les Newell <les.newell@fastmail.co.uk>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

6

I don’t know that you have to have any dwell, most machines can’t move fast enough when reversing, so the tapping head will do it’s pull out and release any way. At least if you are spinning some decent rpm.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 2, 2014, at 8:54 AM, Les Newell les.newell@fastmail.co.uk (les.newell@fastmail.co.uk) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Thanks Brian,I think the main thing missing from SheetCam’s Tapmatic tapping code is the dwell at the bottom.LesOn 02/06/2014 14:36, Brian Lamb > blamb11@cox.net > (> blamb11@cox.net> ) [sheetcam] wrote:

Hi Les,
Sure, but there are several styles of tapping, so I’ll describe what I do in each case. Now, I don’t have rigid tapping so that won’t be a method I know about.

First, this is how I do tapping with “Tension and Compression” style holders, this is where you have to reverse the spindle. The advantage to this style holder is I don’t have to have a torque arm on my mill, which is rather difficult to set up on a moving quill knee mill.

N2010 (1/4-28 tap)
N2020 T6 M06 G43 H6
N2030 M07
N2040 S1000 M03
N2050 G00 X.19 Y-2.75
N2060 Z-1 (my hole surface is down at Z-1.3)
N2070 G01 Z-1.8 F35.7 (feed is 1/28 time the rpm)
N2080 M04 (Reverse the spindle)
N2090 G04 F1 (Dwell for one second, my spindle takes that long to stop and reverse, this varies with rpm)
N2100 Z-1 (feed back out)
N2110 M03 (back to forwards speed)
N2120 G00 Y-.25 (on to next hole and repeat)
N2130 G01 Z-1.8
N2140 M04
N2150 G04 F1
N2160 Z-1
N2170 M03
N2180 G32 (retract to tool change position)


Now, if I use my Tapmatic it goes a little different, I have an NC-1 which reverses at the same speed as forwards. A lot of Tapmatics reverse at 1.5 or 1.75 times the forward speed so increased feedrate would need to be set up.

(1/4-28 tap)
T6 M06 G43 H6
M07
S1000 M03
G00 X.19 Y-2.75
Z-1
G01 Z-1.8 F35.7
G04 F.1 (short 1/10 second dwell to allow the pullout and release)
Z-1
G00 Y-.25
G01 Z-1.8
G04 F.1
Z-1
G32


I don’t go to the trouble to use the tapmatic unless I have like 5 or more holes per part, and I can load the head into the spindle, engage the torque arm and just leave it in the spindle and change the parts in the vise and just do the tapping cycle as a separate operation on my parts. If you have a toolchanger, then you are talking a VMC and they have brackets and such to act as torque arms and will work through a toolchange.

In both cases, I’m allowing for pull out, or over run myself, like I said before, so darn many variables, that’s it’s just easier to program way shallow and then adjust the code and be done with it.

I hope that helps…. let me know if you have any other questions.
Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )

On Jun 2, 2014, at 3:50 AM, Les Newell > les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> ) [sheetcam] <> sheetcam@yahoogroups.com > (> sheetcam@yahoogroups.com> )> wrote:

Hi Brian,
Could you describe your ideal sequence of moves for tapping. I don’t have a tapping head here so I’ve never tested the moves myself.Les

\



.,._
Posted by: Brian Lamb <blamb11@cox.net>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

7

SheetCam’s tapping cycle is based on this document http://tapmatic.com/images/pdf/install_instructions.pdf. The second page cobvers programming. Axial travel in SheetCam is the equivalent to fast retract distance in that document.

Don, you said you were worried about the fast retract stalling your stepper. This shouldn’t happen because Mach always limits the feed rate to the rapid speed. It will never move faster than the G0 speed.

Les


On 02/06/2014 17:15, Brian Lamb blamb11@cox.net (blamb11@cox.net) [sheetcam] wrote:

I don’t know that you have to have any dwell, most machines can’t move fast enough when reversing, so the tapping head will do it’s pull out and release any way. At least if you are spinning some decent rpm.
Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
\



.,._
Posted by: Les Newell <les.newell@fastmail.co.uk>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

8

Les,
To add to the confusion, remember sometime back (a year or two or so), I bought a Tapmatic clone and was having some problems setting it up with Sheetcam. In my case, it was because of the “deadband” of approximately 1/4" between forward and reverse. I don’t remember exactly what I changed in the paramaters (and possibly in my custom post processor), but was able to get it setup and working in a very satisfactory manner. After an incident of a broken tap due to this difficulty and the minor changes I made, I successfully tapped 50 M3 (through) holes in .5" thick 6061 Aluminum.

As previously noted, not all these heads have the same exact parameters. The most obvious is the pullout ratio vs the drive in rate. Then there is the “deadband” region which from past experience runs from a minimum of 0 to in my case .375" on one head that I acquired at a boot sale. One must also make sure the Z axis goes high enough to be sure the tap is fully extracted from the material. This was my main problem due to the “deadband” initially as the tap was not fully extracted before it tried to do the XY move to the next hole.

Hope this may help in your efforts.

Art
Country Bubba

At 12:31 PM 6/2/2014, you wrote:


SheetCam’s tapping cycle is based on this document <> http://tapmatic.com/images/pdf/install_instructions.pdf> >. The second page cobvers programming. Axial travel in SheetCam is the equivalent to fast retract distance in that document.

.,._
Posted by: Art Eckstein <art.eckstein@gmail.com>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

9

I have used G84, but SC doesn’t do canned cycles very well. I also seem to have some issues with my spindle reversing quickly enough. If I write my program out long hand calling for forwards and reverse, I get a much more reliable reverse. I suspect there are parameter settings in the control in regards to the dwell times used in the G84 cycle.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 2, 2014, at 9:42 AM, zrtorres@hotmail.com (zrtorres@hotmail.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Hi…
I have seen this has turned into a large Post…

I use Sheetcam for my Plasma Cutter, but I have Never used Sheetcam to Program a mill…, I also have a CNC Machining Center, and I use another software to generate the G Code for the mill…

This is the Code for a Tapping Cycle I use:

T4 M6
G0 G90 X1.0827 Y-4.0827 S255 M3
G43 Z1. H4 M8
G0 X1.0827 Y-4.0827
G84 G98 X1.0827 Y-4.0827 Z-1. Q0.0625 R0.1 F15.9
X5.2165 R0.1
Y-1.0315 R0.1
X1.0827 R0.1
G80


This cycle is for 4 Holes 3/8"-16, at 255 RPM, and a feed rate of 15.9 IPM. It just basically “synchorinizes” the RPM to the Feed Rate to match the pitch of the thread 3/8"-16.

There is no Dwell Time, and no other paramaters, just goes in, and then, it reverses spindle rotation, and goes out.

For this cycle to work, I MUST use a Floating Tap Holder. If I dared to use a Rigid (NOT Floating) Tapping, the Tap would certainly break, or cause quite some trouble. > Maritool.com > has some different Floating Tap Holders…, I realize these holder are big, but maybe this can guide you in the right direction…

I hope this helps…



\



.,._
Posted by: Brian Lamb <blamb11@cox.net>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

10

G84 requires encoder feedback its a cimplicated canned cycle. I didnt read all the posts but a floating tap holder is the way to go.


-------- Original message --------
From: “Brian Lamb blamb11@cox.net [sheetcam]” <sheetcam@yahoogroups.com>
Date: 06/02/2014 6:14 PM (GMT-06:00)
To: sheetcam@yahoogroups.com
Subject: Re: [sheetcam] Tapping Head setup



I have used G84, but SC doesn’t do canned cycles very well. I also seem to have some issues with my spindle reversing quickly enough. If I write my program out long hand calling for forwards and reverse, I get a much more reliable reverse. I suspect there are parameter settings in the control in regards to the dwell times used in the G84 cycle.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 2, 2014, at 9:42 AM, zrtorres@hotmail.com (zrtorres@hotmail.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Hi…

I have seen this has turned into a large Post…


I use Sheetcam for my Plasma Cutter, but I have Never used Sheetcam to Program a mill…, I also have a CNC Machining Center, and I use another software to generate the G Code for the mill…


This is the Code for a Tapping Cycle I use:


T4 M6
G0 G90 X1.0827 Y-4.0827 S255 M3
G43 Z1. H4 M8
G0 X1.0827 Y-4.0827
G84 G98 X1.0827 Y-4.0827 Z-1. Q0.0625 R0.1 F15.9
X5.2165 R0.1
Y-1.0315 R0.1
X1.0827 R0.1
G80




This cycle is for 4 Holes 3/8"-16, at 255 RPM, and a feed rate of 15.9 IPM. It just basically “synchorinizes” the RPM to the Feed Rate to match the pitch of the thread 3/8"-16.


There is no Dwell Time, and no other paramaters, just goes in, and then, it reverses spindle rotation, and goes out.


For this cycle to work, I MUST use a Floating Tap Holder. If I dared to use a Rigid (NOT Floating) Tapping, the Tap would certainly break, or cause quite some trouble. > Maritool.com > has some different Floating Tap Holders…, I realize these holder are big, but maybe this can guide you in the right direction…


I hope this helps…






\





.,._
Posted by: jeepsr4ever <jeepsr4ever@yahoo.com>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

11

HIYA LES, With a tapmatic you NEED to use the fast retract as described in the manual. This is to ensure that the forward clutch disengages and the reverse clutch ENGAGES correctly . Otherwise clutch dogs do not engage correctly and it may CHATTER going up .

At the TOP of the stroke on retract I slow the Z feed to allow the pressure to come OFF the tap as it pulls OUT of the material . On small taps the pressure can tear the thread as it pulls free of the material.

SAME with ANY compression / Tension device.

Most of the time the normal Tapmatic process works just fine.

Just a thought, (:wink: TP

12

Art, which tapping head do you have. The reason I ask is that I think it would be a good thing for this conversation to have a list of heads and what their specs are. Some of the heads have little available information that I can find on the web, my STM JSN7 is a good example of that I found the setup for 0.14 of self feed in one catalog, I couldn’t find a Mfg/s site on the head.

I’ve been playing with a test bed setup that could give some hard numbers for compression on the down stroke, clutch release and reverse clutch points. There are probably a few more data points that would sort out how to setup your head. I’m absolutely sure there is no one answer as I can’t find much in the way of common traits between my two heads other the a 2X reverse speed. Everything else is different.

Don

.,._
Posted by: Don@Campbell-Gemstones.com

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

13

Don,
I don’t remember the exact name right now, but will go to the shop in
the morning and see what I can find out. I “think” I bought it from
Enco, but don’t make me swear to that. The other one I got was at a
MSC tent sale and I will try to dig out the specks on that one also.

art
Country Bubba

At 08:30 PM 6/3/2014, you wrote:


Art, which tapping head do you have. The reason I ask is that I
think it would be a good thing for this conversation to have a list
of heads and what their specs are. Some of the heads have little
available information that I can find on the web, my STM JSN7 is a
good example of that I found the setup for 0.14 of self feed in one
catalog, I couldn’t find a Mfg/s site on the head.

I’ve been playing with a test bed setup that could give some hard
numbers for compression on the down stroke, clutch release and
reverse clutch points. There are probably a few more data points
that would sort out how to setup your head. I’m absolutely sure
there is no one answer as I can’t find much in the way of common
traits between my two heads other the a 2X reverse
speed. Everything else is different.

Don

_

Posted by: Art Eckstein <art.eckstein@gmail.com>

Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/

14

Don,
A little slow today, but got to the shop and brought the tapping head back to the house so we can try to give pertinent information:
IIRC, I bought this from Enco, but can’t find my shipping info. However it appears to be the same one listed as the “Enco” brand on the current web site.

It is Branded Taco
MFD in India
US parts source http://www.galaxysourcing.com/
Model HR-1
Capacity is 1/16" to 1/4" (and equiv. metric) and comes with two collets and associated wrenches and torque arm
A separate purchase was required to mate the 33JT to R8 to fit my mill
The reverse feed is 1.75 times the down feed
TOTAL stroke length is ~0.46"
Stroke length with the unit collapsed until forward direction hits neutral is approximately .29"
The “neutral” dead band then extends to approximately .34"
The remaining ~.12" is for the reverse feed.

These measurements are probably rough as I was trying to hold the head in one hand and used my thumb to find the different transition areas while measuring with a digital caliper in the other hand:})

When I got the unit, I googled and found a pdf file for their units and if you would like can upload it. Also from their pdf, (hopefully) below is listed their recommended tapping speeds.




HTH and if I have missed anything, let me know.

Art
Country Bubba







At 08:30 PM 6/3/2014, you wrote:


Art, which tapping head do you have. The reason I ask is that I think it would be a good thing for this conversation to have a list of heads and what their specs are. Some of the heads have little available information that I can find on the web, my STM JSN7 is a good example of that I found the setup for 0.14 of self feed in one catalog, I couldn’t find a Mfg/s site on the head.

I’ve been playing with a test bed setup that could give some hard numbers for compression on the down stroke, clutch release and reverse clutch points. There are probably a few more data points that would sort out how to setup your head. I’m absolutely sure there is no one answer as I can’t find much in the way of common traits between my two heads other the a 2X reverse speed. Everything else is different.

Don

.,._
Posted by: Art Eckstein <art.eckstein@gmail.com>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

15

Don,
That’s the exact one! That video is what mine looked like when it did the M3 holes in 6061. Nice and smooth with no problems.
The problem I had setting it up to begin with in Sheetcam was due to the “dead zone” between forward and reverse.





At 03:32 PM 6/4/2014, you wrote:


Art, thanks for the info. While your head is a bit different than my STM head, it seems to handle the tapping the same. From your note, I found this link
Tapping Head
>

Tapping Head
" alt=“Yahoo! Groups” style=“border: 0;”/>
• Unsubscribe (> <sheetcam-unsubscribe@yahoogroups.com>> ?subject=Unsubscribe) • > Terms of Use >

.,._
Posted by: Art Eckstein <art.eckstein@gmail.com>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

16

This is all really useful information. I’ll definitely have to put some
more thought into the tapping routines.

Les

\

Posted by: Les Newell <les.newell@fastmail.co.uk>

Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/

17

Why is there a problem? When your Z axis stops feeding the tapping head continues to feed until it disengages. Then you reverse your Z axis and it engages the reverse feature of the tapping head, and the tap follows the Z axis up and out of the hole. Programming is as simple as knowing the amount of Z pull out and decreasing your overall depth call out by that amount.


Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 4, 2014, at 12:46 PM, Art Eckstein art.eckstein@gmail.com (art.eckstein@gmail.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Don,That’s the exact one! That video is what mine looked like when it did the M3 holes in 6061. Nice and smooth with no problems. The problem I had setting it up to begin with in Sheetcam was due to the “dead zone” between forward and reverse. At 03:32 PM 6/4/2014, you wrote:

Art, thanks for the info. While your head is a bit different than my STM head, it seems to handle the tapping the same. From your note, I found this link > Tapping Head > >
Unsubscribe (> <sheetcam-unsubscribe@yahoogroups.com>> ?subject=Unsubscribe) • > Terms of Use >



.,._
Posted by: Brian Lamb <blamb11@cox.net>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

18

Brian,
When I first tried to use Sheetcam with a tapping head, the first problem was the recognition that the tap would continue to go down as you have noted. The next problem was that with THAT tapping head, was (and I don’t remember why now as that was several years ago) that the tap was driven down to a point that when reversed, it actually pulled the tap out of the head a slight amount. After a couple or three holes, the tap was still in the hole when it tried to move to the next XY position and that = broken tap. As Don has stated, not all of these tapping heads are created equal and you need to know what parameters that need to be adjusted and how to adjust them.

Back when I was trying to learn how to set mine up is when we had a discussion on the group about the “deadband” where the head was turning in neutral (neither up or down on the tap) and found this to be a major variable. I also think this is where the dwell factor came in. Remember, the spindle is always turning so if you stop the down feed AND you have not reached the end of travel (of the tapping head), the tap will continue down. Especially if your doing blind holes, this can be disastrous.

So based on your contention (which is mostly correct), you need to drive the tap down, stop before you have reached full depth, dwell until the tap has stopped rotating and then start the up feed which must also include a necessary amount cover the “dead band” area IF one is present and then make sure you have the tap out of the material before you continue to the next hole.

Art
Country Bubba


At 06:19 PM 6/4/2014, you wrote:


Why is there a problem? When your Z axis stops feeding the tapping head continues to feed until it disengages. Then you reverse your Z axis and it engages the reverse feature of the tapping head, and the tap follows the Z axis up and out of the hole. Programming is as simple as knowing the amount of Z pull out and decreasing your overall depth call out by that amount.


Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )

.,._
Posted by: Art Eckstein <art.eckstein@gmail.com>

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

19

The Idea is to NOT let the spindle drive the tap further down. It should immediately reverse the Z at a fast initial rate to STOP the downfeed from the tap and set the reverse clutch. THen finish the Z upfeed at the proper rate. TO avoid pullout at the top of stroke.

Just a thought, (:wink: TP

20

Brian, a couple problems with how that is handled. When you get to depth, the code assumes you are done moving and goes to the next step. The way the code is now, you go to desired finish depth, then do a jerk back to the axial travel depth while the tap is still trying to pull deeper. You are still under a G01 and G95, so the jerk back F number in the post is 1000, but in the Tap file the F on the Z retract is F393.7008 Not a clue where that number is generated. As the jerk back is taking place, for a portion of it, the tap is still self feeding. In theory, the feed rate on the jerk will get you back into the neutral zone prior to the tap over feeding to much. This isn’t the motion Art and my tap heads were designed to work with

If you study the first vidio in the link I posted and pay attention to the tap holder and the bottom of the tap head, you will see that there is a bit of compression at the start of the hole, IE the tap hasn’t bit and is not feeding it’s self down yet, but the head is feeding. This compression zone is a tad over 1/8" on my head. Now the tap and head progress at the same speed until the head reaches the desired depth + the length of the Axial travel. In my example desired Z depth is 0.500". Axil Travlel, is 0.14 “, so the head should stop is Z- travel at 0.360”. Then no movement should take place of the head until after the self feed is complete. Both Art’s and my heads will accommodate taps from 0-80 up to 1/4-20, so the wait time can be from 3 spindle indexes up to 12 indexes, depending on the TPI being cut. At the end of the dwell, the head will be in the neutral zone and then retract can start.

This is an issue for our type heads, but my Procunier head has a different feed method and none of this applies to it, but the existing code probably wouldn’t work well with it either.

Les, I though I had a possible post fix, but for the life of me, I couldn’t get it to generate anything more than a line F0.0
My though was to change the --retract to engage reverse clutch routine to adding an additional z depth and changing the feed rate to almost zero. As a 0-80 tpi needs 11.8 revolutions to consume the 0.14" I figured that if I inserted EndZ = drillz + tapTravel +0.002 and set a feed rate of 0.0001, that would give a 20 rev pause that would let the tap get into the dead zone, then the retract could take place. I apparently don’t know enough about the post format and more important the term and how they translate to tool input fields. I think I figured out that the post tapTravel is the same a the tool table Axial travel. I also found that although the Mach3 post shows a modifier to feed called underFeed, changing the Underfeed in the tool table has no effect on the output feed rate

I was able to get the actual feed down to the desired drillz + axial travel. The dwell or a method to mimic a dwell are beyond me.

I’m quite obliviously over my head in the coding here.

.,._
Posted by: Don@Campbell-Gemstones.com

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_