Tapping Head setup

[Les Newell les.newell@...]

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/

[Brian L]

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 ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) • Terms of Use

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[art]

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

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Vmax549]

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, (;-) TP

[Don@Campbell-Gemstones...]

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

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Don@Campbell-Gemstones...]

Brian you were on a roll until the last paragraph. With the "ball drive" you have to lingerer at the Zdepth until the tap goes into the dead zone. The Code moves to the next move as soon as the first is satisfied. Although the first is satisfied, the actual travel isn't, until the tapTavel is finished. That is the crux of our problem.

Don

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Steve Blackmore steve@...]

On 04 Jun 2014 18:01:51 -0700, you wrote:

Brian you were on a roll until the last paragraph. With the "ball drive" you have to lingerer at the Zdepth until the tap goes into the dead zone. The Code moves to the next move as soon as the first is satisfied. Although the first is satisfied, the actual travel isn't, until the tapTavel is finished. That is the crux of our problem.

Problem is as you say - how do you know how far your spindle is going to
turn when you command a stop? It depends on the friction of the tap in
the hole amongst other things.

Another problem is that most CNC self reversing tapping heads require
the spindle stops at the same place in it's rotation every time!

Have a read of this

http://tapmatic.com/images/pdf/inst_rdt15-25-50.pdf

it applies to all the CNC clones I'm aware of. The rapid part of the out
move is necessary for some types to engage reverse feed.


However, I do tap using a non reversing floating head NC-1 type tapping
head.

http://tapmatic.com/images/pdf/inst_nc.pdf

On through holes, or blind holes where the thread depth isn't critical I
simply reverse out - no dwell required or tricky code. All feed speeds
on these types are 95% of actual tap pitch.

I do have a manual Tapmatic head too - I use that in the drill press and
it's often much easier just to use that

Ohh - nearly forgot - ALWAYS use proper machine taps!! Spiral point for
through holes, spiral flute for blind holes - or roll form <G>.

Steve Blackmore
--


------------------------------------
Posted by: Steve Blackmore <steve@pilotltd.net>
------------------------------------

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/

[art]

Another thought that I just had is based on the fact that these tapping heads were primarily designed to be used in a drill press or like type of machine. Human reaction time is much slower than a coded cnc machine and as Don points out, results in stresses that the head was never designed to anticipate.



At 08:48 PM 6/4/2014, you wrote:

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


Posted by: Don@Campbell-Gemstones.com

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Brian L]

OK, I’m talking about the process needed and not whatever code results you are getting from SC. I write my own code for tapping, your example would be:

S1000
G00 X0 Y0
Z.3
G01 Z-.360 F31.25
G04 F1
Z.3


You have a one second dwell at the bottom of the hole to allow for the self feed into neutral, this also allows for any compression you got at the beginning of the hole.


I also wouldn’t do the tap cycle in G95, this isn’t rigid tapping, use G94 and calculate the feed rate based on rpm times pitch, that is the way it has been done for the past 35 years or more. You use G95 on a lathe for threading or a mill that has an encoder on the spindle and can rigid tap. The 393.7008 is an inch conversion of a metric number, actually 10,000mm.

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



On Jun 4, 2014, at 5:48 PM, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

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 rateI 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: Brian Lamb <blamb11@cox.net>


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Don@Campbell-Gemstones...]

OK, I’m talking about the process needed and not whatever code results you are getting from SC. I<<

Brian, that code results from SC is the reason for this thread.

Your example cleared up one major point for me though. I had overlooked the G04. If sheetcam can generate a G04, then the P value could be calculated by tap pitch, S, and Axial Travel. After a little more searching in Sheetcam, plasma does have a dwell, so I'm off on another path now to see if I can include a dwell cycle in the post. .

thanks for turning on another light for me.

Don

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Don@Campbell-Gemstones...]

Les, great job. I am not able to test it on the machine right now, but the Gcode looks right on.

IF you created a variable, call it dwellTurns, where dwellTurn = tapTravel / tapPitch, then the minimum dwell time could be derived by dwellTurn / spindleSpeed / 60 This would be the minimum dwell time and probably it should be bumped up by 10% for a little cushion .

Thanks for your help, yet again.

Don

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Les Newell les.newell@...]

In the final version I'll probably calculate the dwell as you suggest, though I will probably allow more than 10%.

Les

On 05/06/2014 23:04, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] wrote:

Les, great job.  I am not able to test it on the machine right now, but the Gcode looks right on. 

IF you created a variable, call it dwellTurns, where dwellTurn = tapTravel / tapPitch,  then the minimum dwell time could be derived by dwellTurn / spindleSpeed / 60   This would be the minimum dwell time and probably it should be bumped up by 10%  for a little cushion .

Thanks for your help, yet again. 

Don

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[art]

Les,
Just to let you know, there are more of us out here that are looking forward to this post!

Art
Country Bubba

At 12:15 PM 6/6/2014, you wrote:

In the final version I'll probably calculate the dwell as you suggest, though I will probably allow more than 10%.

Les

On 05/06/2014 23:04, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] wrote:

Les, great job. I am not able to test it on the machine right now, but the Gcode looks right on.Â

IF you created a variable, call it dwellTurns, where dwellTurn = tapTravel / tapPitch, then the minimum dwell time could be derived by dwellTurn / spindleSpeed / 60  This would be the minimum dwell time and probably it should be bumped up by 10% for a little cushion .

Thanks for your help, yet again.Â

Don

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Brian L]

Les, I ran this post on a job I’m running right now and it had some Z depth issues. I sent a support file to you.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 5, 2014, at 3:09 AM, Les Newell les.newell@fastmail.co.uk (les.newell@fastmail.co.uk) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

This post pauses for half a second at the bottom of the hole. It also stops short of the final depth by the axial travel amount. In other words set axial travel to be the distance from the tap position in free air to the point where it disengages.At the moment the delay is hard coded. You can change it by editing line 259:reverseDwell = 0.5The post is just to test the moves. If it works I will modify SheetCam to make the head type and dwell selectable.Les

<Mach3-tap-dwell.scpost>

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___

[Brian L]

Hi Steve,

Dwell will disengage the tapping sequence, whether it’s a ball drive, friction cone, whatever, you dwell at a set Z and the tap pulls the head into neutral.


Friction of the tap doesn’t effect the depth much, the ball drive style drives until the balls come out of the driven cog… I suppose if the tap had enough inertia to spin a turn or two before it stopped it could be deeper in free-tapping material, but honestly, I don’t see that happening and I’ve used just about every type of tapping head available. Friction drive works the same way, as soon as Z feed stops and the tap walks away from the friction cone, revolutions stop.


Not sure where or why you think a CNC tapping head cares where in the revolution it stops, it stops because of lack of Z feed.


Your first pdf, well, tapmatic says that, I’ve never used that process, I have the N/C-R head as indicated in your second PDF and have used that process on any and all heads I’ve ever used. I see no reason you couldn’t use the rapid out for a certain distant process, but then I see no value in using it either, and I suspicion you take the chance of yanking the tap gradually out of the collet if you go that way.

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



On Jun 4, 2014, at 10:58 PM, Steve Blackmore steve@pilotltd.net (steve@pilotltd.net) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

On 04 Jun 2014 18:01:51 -0700, you wrote:>Brian you were on a roll until the last paragraph. With the "ball drive" you have to lingerer at the Zdepth until the tap goes into the dead zone. The Code moves to the next move as soon as the first is satisfied. Although the first is satisfied, the actual travel isn't, until the tapTavel is finished. That is the crux of our problem. Problem is as you say - how do you know how far your spindle is going toturn when you command a stop? It depends on the friction of the tap inthe hole amongst other things.Another problem is that most CNC self reversing tapping heads requirethe spindle stops at the same place in it's rotation every time! Have a read of thishttp://tapmatic.com/images/pdf/inst_rdt15-25-50.pdfit applies to all the CNC clones I'm aware of. The rapid part of the outmove is necessary for some types to engage reverse feed.However, I do tap using a non reversing floating head NC-1 type tappinghead.http://tapmatic.com/images/pdf/inst_nc.pdfOn through holes, or blind holes where the thread depth isn't critical Isimply reverse out - no dwell required or tricky code. All feed speedson these types are 95% of actual tap pitch.I do have a manual Tapmatic head too - I use that in the drill press andit's often much easier just to use that ;)Ohh - nearly forgot - ALWAYS use proper machine taps!! Spiral point forthrough holes, spiral flute for blind holes - or roll form <G>.Steve Blackmore--

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


Visit Your Group

• New Members 1

Unsubscribe ([email]sheetcam-unsubscribe@yahoogroups.com?subject=Unsubscribe[/email]) &bull; Terms of Use



__,_._,___