Tapping Head setup New Post Problem

Yahoo posts
1

A little more info. I brought up an old job and set the post to Mach3 and ran the post. My Z depths were all good. I then changed the post to Mach3-tap-dwell and re ran the post, My Z moves are all above the work, and this it for drilling and engraving.

This is the start using the Mach3-tap-dwell post where the Z is always a positive number.

N0010 (Filename: Hinges-2.tap)
N0020 (Post processor: Mach3-tap-dwell.scpost)
N0030 (Date:11/06/2014 Time:11:19:15)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: 7128 Door)
N0080 (Operation: No Offset, 7128 Door Text, T7: engraving bit, 0.005 in Deep)
N0090 S8000 G00 Z3.1300
N0100 X0.0000 Y0.0000
N0110 (finish allowance: 0 in)
N0120 (engraving bit)
N0130 T7 M06 G43 H7
N0140 G00 Z0.2550
N0150 S8000 M03
N0160 X1.3718 Y0.6482
N0170 (Fostner bit)
N0180 G01 Z0.125 F5
N0190 F25
N0200 M1104
N0210 G03 X1.3802 Y0.7024 Z0.1250 I-0.0282 J0.0321 F25.0
N0220 M1104
N0230 X1.3467 Y0.7088 I-0.0197 J-0.0122
N0240 M1104
N0250 X1.3360 Y0.6794 I0.0241 J-0.0255
N0260 M1104
N0270 X1.3392 Y0.6608 I0.0453 J-0.0018
N0280 M1104
N0290 X1.3718 Y0.6482 I0.0219 J0.0081
N0300 G00 Z0.2550
N0310 X1.4707
N0320 G01 Z0.125 F5


Then I set the post to Mach3 and re ran the post again and got this which is correct

N0010 (Filename: Hinges-1.tap)
N0020 (Post processor: Mach3.scpost)
N0030 (Date:11/06/2014 Time:11:17:29)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: 7128 Door)
N0080 (Operation: No Offset, 7128 Door Text, T7: engraving bit, 0.005 in Deep)
N0090 S8000 G00 Z3.0000
N0100 X0.0000 Y0.0000
N0110 (Fostner bit)
N0120 (engraving bit)
N0130 T7 M06
N0140 G43 H7
N0150 G00 Z0.1250
N0160 S8000 M03
N0170 X1.3718 Y0.6482
N0180 G01 Z-0.005 F5.0
N0190 F25.0
N0200 G03 X1.3802 Y0.7024 Z-0.0050 I-0.0282 J0.0321
N0210 X1.3467 Y0.7088 I-0.0197 J-0.0122
N0220 X1.3360 Y0.6794 I0.0241 J-0.0255
N0230 X1.3392 Y0.6608 I0.0453 J-0.0018
N0240 X1.3718 Y0.6482 I0.0219 J0.0081
N0250 G00 Z0.1250
N0260 X1.4707
N0270 G01 Z-0.005 F5.0
N0280 G03 X1.4806 Y0.7017 Z-0.0050 I-0.0259 J0.0325 F25.0
N0290 X1.4440 Y0.7086 I-0.0216 J-0.0142
N0300 X1.4324 Y0.6795 I0.0223 J-0.0257
N0310 X1.4356 Y0.6609 I0.0450 J-0.0017
N0320 X1.4707 Y0.6482 I0.0236 J0.0102

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

Visit Your Group

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



,.,_

2

I had though I posted another post this morning before my More info note. I’ve been playing with the new post, and while it seemed to be exactly what I need, all the right moves, something changed and now I can’t seem to get the Z into the stock, Same issue Brian was having a couple days back.

I redownloaded the post to make sure I didn’t screw up something while I was looking at it, but I not only have Z issues on tapping, but with drilling, and engraving. See my two examples in my previous post. Also these examples were run 6.0.5

Don

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

Visit Your Group

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



,.,_

3

Glad to see I wasn’t the only one with problems. It might be easier to copy the tapping section of the post into the existing post you are using.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 11, 2014, at 12:41 PM, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

I had though I posted another post this morning before my More info note. I’ve been playing with the new post, and while it seemed to be exactly what I need, all the right moves, something changed and now I can’t seem to get the Z into the stock, Same issue Brian was having a couple days back.I redownloaded the post to make sure I didn’t screw up something while I was looking at it, but I not only have Z issues on tapping, but with drilling, and engraving. See my two examples in my previous post. Also these examples were run 6.0.5Don

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

Visit Your Group

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



,.,_

4

Hi Les,

Here are the results with the new post, workable, but a few things I still don’t understand. I had the depth called to .75 and the pullout on the tapping head at .188, so that makes sense at Z-.562. The N190 line with Z of 1mm doesn’t make much sense to me as I had the R level at Z.1. The retract to Z.227 is a bit baffling for me too, then back down to Z.1?







N0010 (Filename: Tap test 2.tap)
N0020 (Post processor: Mach3-tap-dwell.scpost)
N0030 (Date:12/06/2014 Time:08:44:57)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: Indicator op10)
N0080 (Operation: Tap, CENTER, T24: 1/4-20 tap, 0.75 inch Deep)
N0090 S1000 G32
N0100 X-20 Y05
N0110 (finish allowance: 0 inch)
N0120 (1/4-20 tap)
N0130 T24 M06 G43 H24
N0140 M07 (Mist coolant on)
N0150 S1000 M03
N0160 M49
N0170 G95
N0180 G00 X1.5000 Y-1.2601
N0190 Z0.0394
N0200 G01 Z-0.562 F0.047
N0210 G04 P0.5
N0220 Z0.227
N0230 G00 Z0.1000
N0240 M48
N0250 G94
N0260 X8.0000 Y3.0000
N0270 M09 (Coolant off)
N0280 M05
N0290 M05 M30




On Jun 12, 2014, at 1:47 AM, Les Newell les.newell@fastmail.co.uk (les.newell@fastmail.co.uk) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

<Mach3-tap-dwell.scpost>


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

Visit Your Group

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



,.,_

5

Hi Brian,

The 1mm is a safety clearance height before is starts to plunge. This is like the plunge safety clearance but fixed at 1mm at the moment. It rapids to position at the clearance plane, drops to 1mm then starts tapping. Could I just use the plunge safety clearance here?

The retract to Z.227 is because the tap is now extended as the head is in reverse mode. You need to retract high enough for the extended tap to pull out of the hole. At least I think that is how the head operates.

Les


On 12/06/2014 16:54, Brian Lamb blamb11@cox.net (blamb11@cox.net) [sheetcam] wrote:

Hi Les,

Here are the results with the new post, workable, but a few things I still don’t understand. I had the depth called to .75 and the pullout on the tapping head at .188, so that makes sense at Z-.562. The N190 line with Z of 1mm doesn’t make much sense to me as I had the R level at Z.1. The retract to Z.227 is a bit baffling for me too, then back down to Z.1?







N0010 (Filename: Tap test 2.tap)
N0020 (Post processor: Mach3-tap-dwell.scpost)
N0030 (Date:12/06/2014 Time:08:44:57)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: Indicator op10)
N0080 (Operation: Tap, CENTER, T24: 1/4-20 tap, 0.75 inch Deep)
N0090 S1000 G32
N0100 X-20 Y05
N0110 (finish allowance: 0 inch)
N0120 (1/4-20 tap)
N0130 T24 M06 G43 H24
N0140 M07 (Mist coolant on)
N0150 S1000 M03
N0160 M49
N0170 G95
N0180 G00 X1.5000 Y-1.2601
N0190 Z0.0394
N0200 G01 Z-0.562 F0.047
N0210 G04 P0.5
N0220 Z0.227
N0230 G00 Z0.1000
N0240 M48
N0250 G94
N0260 X8.0000 Y3.0000
N0270 M09 (Coolant off)
N0280 M05
N0290 M05 M30




On Jun 12, 2014, at 1:47 AM, Les Newell > les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> ) [sheetcam] <> sheetcam@yahoogroups.com > (> sheetcam@yahoogroups.com> )> wrote:

<Mach3-tap-dwell.scpost>

\



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

Visit Your Group

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



,.,_

6

I see…. the retract is .188” plus 1mm, now that makes sense. I would use the safety level or even higher, most tap head builders recommend at least .300” of feed before you hit the hole. If I was using a G84 tapping cycle, I would set my R level to be .3 instead of .1 like I would normally do with a drill. It would be nice if we could put a positive number in the start position and have it be that much above Z0…… if that could/would work.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)



On Jun 12, 2014, at 9:39 AM, Les Newell les.newell@fastmail.co.uk (les.newell@fastmail.co.uk) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Hi Brian,The 1mm is a safety clearance height before is starts to plunge. This is like the plunge safety clearance but fixed at 1mm at the moment. It rapids to position at the clearance plane, drops to 1mm then starts tapping. Could I just use the plunge safety clearance here?The retract to Z.227 is because the tap is now extended as the head is in reverse mode. You need to retract high enough for the extended tap to pull out of the hole. At least I think that is how the head operates.LesOn 12/06/2014 16:54, Brian Lamb > blamb11@cox.net > (> blamb11@cox.net> ) [sheetcam] wrote:

Hi Les,
Here are the results with the new post, workable, but a few things I still don’t understand. I had the depth called to .75 and the pullout on the tapping head at .188, so that makes sense at Z-.562. The N190 line with Z of 1mm doesn’t make much sense to me as I had the R level at Z.1. The retract to Z.227 is a bit baffling for me too, then back down to Z.1?



N0010 (Filename: Tap test 2.tap)
N0020 (Post processor: Mach3-tap-dwell.scpost)
N0030 (Date:12/06/2014 Time:08:44:57)
N0040 G20 (Units: Inches)
N0050 G40 G90 G91.1
N0060 F1
N0070 (Part: Indicator op10)
N0080 (Operation: Tap, CENTER, T24: 1/4-20 tap, 0.75 inch Deep)
N0090 S1000 G32
N0100 X-20 Y05
N0110 (finish allowance: 0 inch)
N0120 (1/4-20 tap)
N0130 T24 M06 G43 H24
N0140 M07 (Mist coolant on)
N0150 S1000 M03
N0160 M49
N0170 G95
N0180 G00 X1.5000 Y-1.2601
N0190 Z0.0394
N0200 G01 Z-0.562 F0.047
N0210 G04 P0.5
N0220 Z0.227
N0230 G00 Z0.1000
N0240 M48
N0250 G94
N0260 X8.0000 Y3.0000
N0270 M09 (Coolant off)
N0280 M05
N0290 M05 M30


On Jun 12, 2014, at 1:47 AM, Les Newell > les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> ) [sheetcam] <> sheetcam@yahoogroups.com > (> sheetcam@yahoogroups.com> )> wrote:

<Mach3-tap-dwell.scpost>

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

Visit Your Group

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



,.,_

7

Les and Brian, This code looks better. As far as the over travel on retract, I think this may need some research. What I’m concerned with the the underfeed. My JSN7 has a considerable amount of reverse engagement, and I would like to make sure I’m not in the neutral zone and the tap is still engaged in the work at the time the rapid to safe height is started. I guess if you set your Rapid Clearance to Axial travel + a little bit, that should ensure the tap is clear.

I’m kind of getting used to one blurry eye, so I’ll go out to the shop and document the two heads I have The JSN7 will take some compression, apx 1/8" After the reverse is engaged, there is some float in the Z+ range, but it looks like when the reverse is engaged, the engagement is maintained well up into what was the neutral zone on the feed stroke.

Don

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

Visit Your Group

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



,.,_

8

Hi Brian,

You can use a negative start depth. This will start above the top of the work.

Les

On 12/06/2014 19:20, Brian Lamb blamb11@cox.net (blamb11@cox.net) [sheetcam] wrote:

I see…. the retract is .188” plus 1mm, now that makes sense. I would use the safety level or even higher, most tap head builders recommend at least .300” of feed before you hit the hole. If I was using a G84 tapping cycle, I would set my R level to be .3 instead of .1 like I would normally do with a drill. It would be nice if we could put a positive number in the start position and have it be that much above Z0…… if that could/would work.
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



,.,_

9

Hi Don,

Hmm, I need to think on that one. I could add an extra parameter to set the amoutn of retract but I don’t want to make it too complicated.

Les

On 12/06/2014 21:09, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] wrote:

Les and Brian, This code looks better. As far as the over travel on retract, I think this may need some research. What I’m concerned with the the underfeed. My JSN7 has a considerable amount of reverse engagement, and I would like to make sure I’m not in the neutral zone and the tap is still engaged in the work at the time the rapid to safe height is started. I guess if you set your Rapid Clearance to Axial travel + a little bit, that should ensure the tap is clear.Â

I’m kind of getting used to one blurry eye, so I’ll go out to the shop and document the two heads I have The JSN7 will take some compression, apx 1/8"Â After the reverse is engaged, there is some float in the Z+ range, but it looks like when the reverse is engaged, the engagement is maintained well up into what was the neutral zone on the feed stroke.

Don


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

Visit Your Group

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



,.,_

10
<?xml version="1.0"?>
11

Les, I think we are making this way more complicated than it is for the Tapmatic/Clones heads. First, without any tension or compression, the tap head is in forward drive. The following measurements are referenced to this point as Z=0 On my head, you can over compress as much a 0.175" before a hard stop in travel. You can under feed by as much as 0.140" and the tap will still find its own way. As along as the feed and rpms are reasonably close, there is no issue.

Now, when the Z stops moving, the tap will continue turning and consume that -0.140" self feed and go into neutral. When the Z+ move starts, the head remains in neutral until it reaches -0.065" at which point, reverse engagement starts. You can overfeed the return as much as 0.250" without trying to pull the tap from the head.

So, the Z moves would look like this
Rapid to hole, at safe height.
Feed to -Z depth + 0.14" (self feed)
Pause
Retract at 2x feed rate and at -Z depth + 0.075", the reverse clutch engages and stays engaged until the tap clears the hole at which point, it will snap the remaining 0.075" up to the head resting point. By my figures, the machine Z has to go to Z+0.215 or the reverse clutch will disengage and leave the tap still in the hole. Brians suggestion of 0.300" is probably a good number to build in. My .125 safe wouldn’t work.

Also, with the long cushion in both feed and retract, and exact match of spindle speed and feed isn’t required, I’m not sure what the wiggle room there is. It will vary with tap pitch.

The Procuiner head is a different story though. There is no cushion on feed clutch or reverse clutch engage. The only cushion is the approximately 1/8" netural zone between the two. The head is spring loaded to keep the forward clutch engaged with no compression on the tap.

I uploaded a photo of my “test Bed” On the right is my 45lb drill press vise standing on it end. It is holding a 1/4" open end wrench which is engaging a flanged bearing on a #4 tap. Below the bearing is a t nut with the small end up to ride the inner race and a lock nut. My kludge of stacking angle plates and 1 2 3 blocks let me measure the travel of the quill and I was turning the top pulley by hand. It was the only methiod I could come up with to get the reverse measurements. I think my translations of my readings are correct. Although I know they are not precise. Some may be a much as 0.010" off the actual.

Don

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

Visit Your Group

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



,.,_

12

Hi Don,

Sorry about the late reply.

So, the Z moves would look like this
Rapid to hole, at safe height.
Feed to -Z depth + 0.14" (self feed)
Pause
Retract at 2x feed rate and at -Z depth + 0.075", the reverse clutch
engages and stays engaged until the tap clears the hole at which
point, it will snap the remaining 0.075" up to the head resting
point. By my figures, the machine Z has to go to Z+0.215 or the
reverse clutch will disengage and leave the tap still in the hole.
Brians suggestion of 0.300" is probably a good number to build in. My
.125 safe wouldn’t work.

That is close to how that experimental post works. The only real
difference is that it retracts to clearance plane + self feed (clearance

  • 0.14" in your case).

The Procuiner head is a different story though. There is no cushion on
feed clutch or reverse clutch engage. The only cushion is the
approximately 1/8" netural zone between the two. The head is spring
loaded to keep the forward clutch engaged with no compression on the tap.

So basically we need two parameters:
Forward disengagement distance. This is the distance the tap will keep
moving after you stop feeding Z. For the Procunier this would be
virtually 0.
Reverse engagement distance. This is the distance Z needs to retract to
engage reverse.

I uploaded a photo of my “test Bed”

Thanks for going to that much effort.

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/

13

Les, no worry about a slow response. All last week was eye drops in prep for yesterdays cataract surgery on my right eye yesterday and it will be another two weeks at best before I can get new glasses to put my vision back to sorta normal and start doing some work again…

Your last post looked like it would solve the issues with my type head, and give me the ability to modify it for my unique head. I would suggest consulting with Brian about the non reversing heads he uses, although I think the only difference between them and the Procniner head will the the stop and motor reverse, and maybe the reverse retract speed. Humm Three different head major types??? Self feeding /self reversing, Self reversing, tension / compression.

Thanks again for all your efforts on this

Don

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

Visit Your Group

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



,.,_

14
<?xml version="1.0"?>
15

Brian, thanks for the input. During all this conversation, this little nagging point kept creeping into my head. As you point out, the tap doesn’t start cutting at z-0.001 but at a variable depth depending on hole size and taper of the tap. One of the reasons I bough the Tapmatic clone was so I could make a couple hundred 0-80 thread turnbuckles. I realized yesterday that I can’t use it for that purpose as the auto feed is going to be deeper than my thread depth. What I need is a 1E Procuiner. This sure has been an education. Thanks for your help.

Don

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

Visit Your Group

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



,.,_

16
<?xml version="1.0"?>
17

Les, I managed to get the spindle index pickup working today. New CNC4PC BOB and some creative wiring to get 5V power to the hall effect and my Tachometer. Now to learn how to setup Mach3 to read the hall effect. I know my wiring is OK, I mistakenly put the pickup on Pin 10 and found as soon as I started the spindle motor, I triggered an EPO. Corrected that but still am unable to get a tach readout. A little investigation on google came up with a long list of things to do, none of which I did, so I’ve a bit of work to do tomorrow. Hopefully before the day is done, I’ll get to try the post mod you did and cut some real threads.

Don

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

Visit Your Group

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



,.,_

18

Progress Report

Good news. I have Mach3 reading my spindle speed, and it matches the DRO that I setup on the spindle it’s self.

I did a test drawing of four dots and set up a job to tap those four dots… When I tried to do some air cutting, Mach3 hung on Line 2 of the tap, Turns out when I was saving the different post, windows was appending a version on the name. Mach3 didn’t like that comment in the tap file Imbedded comment
N0020 (Post processor: Mach3-tap-dwell(2).scpost) so I changed it to
N0020 (Post processor: Mach3-tap-dwell.scpost) and all was well.

While I don’t have Mach actually control the speed, next project, the motor start and speed setting showed in the Mach3 screen and the mach 3 spindle speed matched my tach.

I started an air cut and all went as I expected. I had manually set the speed to 500 rpm and while the z moves seemed a little slower than I expected, it looked OK. I then kicked up the speed to 1500rpm and I didn’t really notice a change is Z speed. I then turned off the spindle and re ran the job, expecting that it would hang on the first Z feed after the G95. It didn’t, it fed the Z at the same speed as when the motor was running. I am researching Mach 3 setup now to find out what is wrong. I at first though it might be using the 500rpm in the S command vs the index pulse, so I changed it to 1500 but it didn’t effect the speed of the feed either.

I suspect that there is a box I didn’t check in Mach3 config that is the problem, now to find it.

Don

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

Visit Your Group

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



,.,_

19

Don,

I don’t know a whole lot about Mach 3, but I was under the assumption it doesn’t do G95 in conjunction with the spindle rpm. Now, I just read the “manual” and it says it can, but I don’t think I’ve heard of many getting it to work correctly on a mill. My thought would be to use G94 and program your feedrate based on rpm x pitch. I suspect you will find your Z axis feedrate keeping up as it should then, at least if it’s capable of moving fast enough. A 1/4-20 thread at 1000 rpm is 50ipm and some stepper driven machines don’t move that fast.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Jun 22, 2014, at 11:27 AM, Don@Campbell-Gemstones.com (Don@Campbell-Gemstones.com) [sheetcam] <sheetcam@yahoogroups.com (sheetcam@yahoogroups.com)> wrote:

Progress ReportGood news. I have Mach3 reading my spindle speed, and it matches the DRO that I setup on the spindle it’s self. I did a test drawing of four dots and set up a job to tap those four dots… When I tried to do some air cutting, Mach3 hung on Line 2 of the tap, Turns out when I was saving the different post, windows was appending a version on the name. Mach3 didn’t like that comment in the tap file Imbedded commentN0020 (Post processor: Mach3-tap-dwell(2).scpost) so I changed it toN0020 (Post processor: Mach3-tap-dwell.scpost) and all was well.While I don’t have Mach actually control the speed, next project, the motor start and speed setting showed in the Mach3 screen and the mach 3 spindle speed matched my tach.I started an air cut and all went as I expected. I had manually set the speed to 500 rpm and while the z moves seemed a little slower than I expected, it looked OK. I then kicked up the speed to 1500rpm and I didn’t really notice a change is Z speed. I then turned off the spindle and re ran the job, expecting that it would hang on the first Z feed after the G95. It didn’t, it fed the Z at the same speed as when the motor was running. I am researching Mach 3 setup now to find out what is wrong. I at first though it might be using the 500rpm in the S command vs the index pulse, so I changed it to 1500 but it didn’t effect the speed of the feed either.I suspect that there is a box I didn’t check in Mach3 config that is the problem, now to find it.Don



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

Visit Your Group

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



,.,_

20

Brian, I read a lot of weird stuff today about G95 and Mach3. All the way from best thing since sliced bread to worst idea yet. One thing popped out that caught my attention. It was a comment that once the move had started, it no longer monitored the index, but fed at the speed that was detected when the move started. If I’m remembering that post correctly, it states it is the same for the mill and turn. That would say that if your spindle got sluggish going into a tap or thread cycle, it may well overfeed as the feed was set as soon as the z move started, even though the tap or tool wasn’t in the work yet.

This has been an interesting problem.

I was already to test it on some aluminum when I realized I hadn’t made a lock for the reverse arm yet. I’ll probably get that finished tomorrow and the try to tap some holes.

Don

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

Visit Your Group

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



,.,_