M05 M06 M03 Problems in Turn

[Liberty FLHTC]

After searching the forum for a few days and not finding an answer, I decided it was time to post.

I sold my brother an engine lathe that had been retro-fitted with steppers to run the carriage lead screw and the cross slide lead screw plus a VFD for spindle RPM control. I used this lathe for several years and never had the following problem surface.

He had written a new program and began having feed rate problems after a tool change. I checked his program and it appeared OK (I even re-typed it into a blank Notepad page in case something was hiding). The program starts out using T0101 with a feed rate of .012 IPR. The feed rate is fine until the first tool change. Here's a clip of the tool change part of the program:

M05
M06 T0202
M03

When tool 2 reaches the first G01 line the feed rate drops to .004 IPR and stays there until the next M05. After the tool change to T0303 the same thing happens. When the M05 is passed at the end of the program the feed rate jumps back to .012 IPR. This feed rate change is visible on the Feed DRO and it can be easily seen when watching the rotation speed of the lead screws.

I've been all through the settings, tried different CV Tolerances, Exact Stop, Plasma on, checked the macros, you can just about name it and I looked at or tested it during the search for the cure. The M05 macro is DoSpinStop() , the M03 macro is DoSpinCW() and the M06Start macro is:
  tool = GetSelectedTool()
  SetCurrentTool( tool )

The programs I had been using mostly have the M06 as a stand alone since I moved the tool post away from the spindle to perform a tool change. There is one area in my programs that has a M05 followed by a M06 then several lines of movement before the M03 command and these have never caused this problem to surface.

He adjusted the program to move the tool holder away from the spindle before tool change, removed the M05 and M03 lines from before and after the M06 line, and the problem disappeared. .012 IPR all the way through.

Anyone have any ideas or cures?

[Liberty FLHTC]

It's been 5 days since I posted this with 30+ views but no responses. I guess the problem either stumped everybody, I somehow made everyone upset, or the solution is obvious and I'm an idiot.

[RICH]

None of the above in reply # 1......you just need to waite for someone who uses a tool changer on their lathe and has experience
on it's use. I don't so can't be of much help.
RICH

[Hood]

I missed this, not sure how as I tend to read all posts on the General forum
I have not seen these issues and I have a twin turret lathe so do plenty tool changes.
If you attach your xml, some code and the complete macro folder for the profile you are using maybe the issue can be found. Also what version of Mach?
One other thing, what does the rpm look like in Mach after tool changes?
Hood

[Graham Waterworth]

I replied to this post but for some reason the reply got deleted.

Here is the reply:-

[Liberty FLHTC]

It may be a couple days before I can get back to this lathe as it is 35 miles away and was just there last evening.

The Mach version we are using is R3.043.022 - same as on my new lathe.

For clarification, after the M06 line the tools are manually indexed on the cross slide with the exception of the cut off as it is mounted on the rear post. The program references the front post all the way through and we use a big offset with negative X values to perform the T0303 cut off operation (same as had been done in my programs).

The spindle RPM remains constant with the exception of turning off and on for the tool change. This was being done as a safety issue to eliminate the chance of inadvertently having a tool contact the rotating spindle during tool change.

This is all relatively new to my oldest brother and thankfully he is using these issues as a learning tool to become accustom to the lathe, the program, and the controls. He runs a range of materials - from plastic to 416 Stainless on this lathe whereas I only ran aluminum and brass. Before he purchased the lathe we set it up to cut and thread a 1" NPT fitting and it worked great.

The replies and help are much appreciated!

[Hood]

Ok this part may be the problem

The spindle RPM remains constant with the exception of turning off and on for the tool change. This was being done as a safety issue to eliminate the chance of inadvertently having a tool contact the rotating spindle during tool change.

If you are in feed per rev and have not got a spindle delay it may be possible that the spindle has not cranked up to is commanded speed when Mach looks at the RPM to work out the feedrate and thus it moves slower.
Try putting a 2 second delay in for the spin up and see if it helps, you can fine tune later if it helps.
I may be way off with this but it just does seem it could be the problem, if its not then nothing lost .
Hood

[Liberty FLHTC]

Hi All!
I'll be going to my brother's to get that info Tuesday evening.

In the meantime, I discovered my lathe pulling the same trick! Attached is the program and the .xml from my lathe.

Everything performs great until it gets to tool t1717. When the g01 line is read the feed rate DRO starts at .012 and quickly drops back to .007.
When t0101 is called next and the g01 line is read, the feed rate DRO reflects the .003 rate. The spindle RPM remains stable throughout the program and performs as directed.

I had m06 in front of the tool change lines and took them out trying to determine if that was the culprit - but NO, that wasn't it.

This one has me scratching my head!!!!!!!!! Any ideas or thoughts?

[Liberty FLHTC]

The forum wouldn't let me load the .txt file, so here it is:

(Use 5/8 2024 Alum. Stock)
g95 g18 f.003 s2000
t0101
g0 x.400 z.375
(feed Bar)
m01
g0 z.400 x.425
m03
g04 p.5
g0 x.425
g01 z0
g0 x.450
g0 z.400
g0 x.275
g01 z.200 f.004
g0 x.425
g0 z0
g01 x.382
g01 z.189
g01 x.377 z.194
g01 x.245
g01 z.325
g01 x.205 z.345
g01 x0
g0 z.600
t1313
g0 x0 z.400
g01 z.280
g0 z.600
t1414
g0 x0 z.400
g01 z.245
g04 p.05
g01 z.145
g04 p.05
g01 z.070
g04 p.05
g01 z0
g04 p.05
g0 z.600
t1515
g0 x.263
g0 z.250
g01 z.150 f.003
g0 z.250
g01 x.251
g01 z.150
g0 z.600
s800
t1616
g0 x.300
g0 z.250
g04 p.5
g01 z.189 f.005
g04 p.02
g01 z.160 f.010
g04 p.02
g0 z.600
m05
m08
t0202
g94
g0 x-.300
g0 z.167
m01
g01 x .050 f2
g0 x-.600
g0 z1.500
m09
m01
m03 s2000
g95 g18 f.012
t1717
g0 x0
g0 z.400
g01 z0
g0 z.6
t1515
g0 x.230
g0 x.258
g0 z.250
g01 z.151 f.003
g0 z.600
t0101
g0 x.382
g0 z.220
g01 z.020 f.004
g01 x.342 z0
g0 x.625
g0 z2.000
m07
g0 a.600
g01 a.100 f.0025
g01 a-.080 f.0015
m09
g0 a2
m05
m30

[Hood]

Try with a G4P2 on the line before the T1717 and see if there is a difference.
Just curious here, I notice you use a lot of tools but dont have an auto changer and there are no M1's before the change so just curious if its the same tool just using different offset?

Hood