tool threading tool doing wierd things

All info relating to the Denford Mirac lathes

Moderators: Martin, Steve, Mr Magoo

Post Reply
KBrown
Posts: 7
Joined: Tue 04 Sep , 2012 2:09 am

tool threading tool doing wierd things

Post by KBrown » Thu 08 Nov , 2012 0:03 am

Hi all.

I’m pretty new to CNC turning and the Denford software.
I’ve pretty much got to grips with setting up material offset, and using a RHK to turn basic items.

I’m now looking at threading but i seem to be having a major problem.
I don’t know whether it is something I’m doing wrong so ill run through what I’m doing step by step, and maybe you can see where I’m going wrong.

Essentially I’m testing turning a piece of parallel 14mmOD bar to M14x1mm before adding it to a more complex shape

the RHK faces the bar and barely skims the 14 stock nicely, however when the external threading tool is selected, the tool goes to the material face origin, and then just plunges in the -ve:X (thats correct – X, not Z), direction, up until it hits the limit switch/or i press emergency stop.
short VIDEO from after the ATC changes to tool #3
>>>>>>>>> https://dl.dropbox.com/u/77961576/denford/DSCF6064.AVI

>>>>>>>>>During the simulation in VRMilling it simulates fine:
https://dl.dropbox.com/u/77961576/denford/1.JPG

>>>>> i cannot attache a .LCM file but if youd like it please let me know and ill email it.

*******

below is a summary of what i do.
I’m using Quickturn2D, and VRturning (current versions)


1) creating the profile in QT2d
threading tool is in position 3
https://dl.dropbox.com/u/77961576/denford/9.jpg
https://dl.dropbox.com/u/77961576/denford/10.jpg

2) load the .fnl file to VRturning

3) set the stock offset by moving tool #1 to the z face of the bar stock – leave as is and clicked ok.
https://dl.dropbox.com/u/77961576/denford/2.JPG
program sets to 0.005
https://dl.dropbox.com/u/77961576/denford/3.JPG

4) then the stock X offset by setting diameter to 14mm and then OK.. – “programme - X’ sets to 14.000 on DRO
https://dl.dropbox.com/u/77961576/denford/4.JPG

5) tool 1 X offset - -tool set to touch ourside of stock, and dia value set to 14 (distance to origin not touched)
https://dl.dropbox.com/u/77961576/denford/5.JPG
6) tool 1 y offset – tool set to touch z face of bar and ok’d
https://dl.dropbox.com/u/77961576/denford/6.JPG

7) then tool 3 – the external threading called up on the ATC and jogged to following position:
https://dl.dropbox.com/u/77961576/denford/DSCF6061.JPG

Tool#3 ‘z’ offset - nothing changed and OK’d
https://dl.dropbox.com/u/77961576/denford/7.JPG

tool # 3 ‘x’ offset diameter set to 14mm
https://dl.dropbox.com/u/77961576/denford/8.JPG

thanks
Keith

Martin
CNC Guru
CNC Guru
Posts: 1897
Joined: Fri 24 Feb , 2006 17:09 pm
Location: Brighouse

Re: tool threading tool doing wierd things

Post by Martin » Thu 08 Nov , 2012 1:44 am

I would set all values for tool 3 back to zero then reset the offsets.

User avatar
Denford Admin
Site Admin
Posts: 3632
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: tool threading tool doing wierd things

Post by Denford Admin » Thu 08 Nov , 2012 10:56 am

The threading codes output by Quickturn 2D will only work on newer machines.
If ever asked to provide QuickTurn for an older Denford lathe, threading is the one thing we say will not work.
The older Lathes will not be able to process the thread g-codes as it worked in a different way.
You would have to manually alter the gcode to match a thread that the older machines can understand, eg:
G76 P050060 Q035 R.05
G76 X18.00 Z-26.5 P1000 Q070 F1.5

as opposed to the newer:
G32X9.342Z-10F0.500

KBrown
Posts: 7
Joined: Tue 04 Sep , 2012 2:09 am

Re: tool threading tool doing wierd things

Post by KBrown » Thu 08 Nov , 2012 16:04 pm

Thanks for the reply guys.

I forgot to mention im running a Mirac-PC - on WinXP
is this an 'older' machine as described above ??

Before i bought QT2D (two week or so ago), i used "Lathecam designer" to produce a part with a thread
https://dl.dropbox.com/u/77961576/denfo ... 20Copy.JPG

Ive just found the code for that and taken a screenshot.
the thread is standard metric M10.

https://dl.dropbox.com/u/77961576/denford/untitled1.JPG

from the code changing to tool#3 it reads:

N184M6T0303
N185G97M3S350
N186G0X11Z5
Continued on screenshot... https://dl.dropbox.com/u/77961576/denford/untitled1.JPG


It looks as if the code is the newer type, can you please confirm..

if it is the older stye of code, then luckily most threads i'll be doing are M14x1 clockwise and M14x1 CCW.

as an example or so i can test, would it be possible if can you please give what i need to substitute for a m14x1 cw external thread, in say 0.25mm incremental steps, as im pretty much new to CNC and im certaily not at the stage of being able to programme without a template.

regards

User avatar
Denford Admin
Site Admin
Posts: 3632
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: tool threading tool doing wierd things

Post by Denford Admin » Thu 08 Nov , 2012 16:28 pm

Yes the Mirac control doesn't know what to do with the newer G32 threading codes.
I'd just draw the thread you want in LatheCAM and copy+paste that into the the section of the QuickTurn program.

Take the bits of program from LatheCAM at the toolchange position and paste them over the threading section.
eg:
replace something like this from quickturn:

Code: Select all

(External Threading Operation)
M06T0303
G97M03S350
G98F250
G00X5Z-0.152
G01X2.474F250
G32X2.474Z-10F0.500
G00X5
G00Z-0.190
G01X2.342F250
G32X2.342Z-10F0.500
G00X5
G00Z-0.190
G01X2.342F250
G32X2.342Z-10F0.500
G00X5
G00Z-0.190
G01X2.342F250
G32X2.342Z-10F0.500
G00X5
G00Z-1
M05
with something like this from LatheCAM:

Code: Select all

M06 T0303 
G97 S350 M03 
G00 X20.5 Z-10 
G76 P050060 Q035 R.05 
G76 X18.00 Z-26.5 P1000 Q070 F1.5 
M05

KBrown
Posts: 7
Joined: Tue 04 Sep , 2012 2:09 am

Re: tool threading tool doing wierd things

Post by KBrown » Thu 08 Nov , 2012 19:24 pm

ok cool, at least you’ve found the fault, and letting me know how to work around it.


bit of an update..

I’ve made a 13,8mm dia male thread on LCD, and broke it down using limited knowledge/Wikipedia


please help me out with any ???’s, as it looks like I'm going to need a crash course on how to define my own thread (dia/pitch/direction)

ive played about in LCD, and made a code for a 13.8mmDIA CW male stud, 25mm long, and got:

M6T0303
G97M3S350
G0X14Z5
G76P036060Q61R0.03
G76X10.854Z-26.5R0P1073Q260F1.75
M5

^^^ broken down from what I understand

M6T0303
>Tool change - tool#3, offset#3

G97M3S350
>G97 - CSS
>M3s350 - Spindle on (CW) @ 350 rpm

G0X14Z5
>G0 = rapid position to:
>x14z5= coordinates x14,z5

G76P036060Q61R0.03
>G76 = threading cycle for turning.
>P 036060 = ????????????????????????????????????????????????????
>Q61 = Peck increment in (61=??????????????)
>R0.03 = radius 0.03?????????????????????????????????

G76X10.854Z-26.5R0P1073Q260F1.75
>G76 = Fine boring cycle for milling ?????????????????????
>x10.854, z-26.5 =
>R0 =0 radius ?????????
>P1073 = parameter 1073 ?????????????
>Q260 = peck increment 260 (what does 260 mean???)
>F1.75 = feedrate 1.75

M5
> spindle stop



*********
as you can see there are a lot of ??? which seem quite important
if you can help me out to understand it and enable me to type my own threads.

from what I understand LCD only does standard metric course pitches, so for example M14x1 will be impossible on it, soi cannot 100% rely on it, as i need to change parameters manually


I found this page on the internet, but I doubt it will be useful as there are codes on it that were not outputted from LCD.( explains G78 coding)
http://www.welsoft.co.uk/machlathe/hs380.htm
if I use that format will the mirac-pc I have understand that type of coding? (ill try it out tomorrow)

Lastly, (and sorry for all the questions), but would you (denford) consider doing a revision in QT2d to have a tickbox to output G76 style coding instead of G32, as I'm sure I'm not the only person having this problem,

thanks in advance
Keith

User avatar
Denford Admin
Site Admin
Posts: 3632
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: tool threading tool doing wierd things

Post by Denford Admin » Fri 09 Nov , 2012 13:07 pm

Go to Help > CNC Programming in VR Turning, this shows you help on all (well, most) of the G codes,eg:
The G76 command contains, within two blocks, all the information required to generate a standard thread form and pitch.
A G76 uses one edge cutting to reduce the load on the tool tip.
Click here to show G76 Canned Cycle General Diagram.
A G76 command is written in the following format:
G76 P (A) / (B) / (C) Q (Min) R ;
G76 X(U) Z(W) P (DEP) Q (1st) F ;
where,
P (A) is the number of thread finishing passes (1 to 99).
P (B) is the chamfer amount. This is the angle at which the tool leaves the billet, at the end of the thread cutting cycle.
P (C) is the angle of the tool tip (8Ø°, 6Ø°, 55°, 3Ø°, 29° and Ø°). Note - (A), (B) and (C) are all specified at the same time by the address P, eg, PØ36Ø6Ø = number of cuts is Ø3, chamfer amount of 6Ø and tool angle of 6Ø°.
Q (Min) is the minimum cutting depth (in microns). When the depth of the cut calculated by the CNC control becomes less than this limit, the cutting depth is clamped at this minimum value.
R is the finishing allowance. This is the final, or finishing, cuts applied to the thread. The number of stages to complete this finishing allowance is determined by the value of P(A), ie, the value of R divided by the P(A) number of finishing passes equals the value of each finishing allowance stage.
X(U) is the end position of the thread in the X axis (the core diameter).
Z(W) is the end position of the thread in the Z axis.
P (DEP) is the depth of the thread as a radius value (in microns).
Q (1st) is the depth of the first pass as a radius value (in microns).
F is the size of the thread pitch.
The Parameter values may look strange, but that's because they are in Microns..so 260 is 0.26mm
Just be aware that the threading cycle on the older machines tended to do it's own thing, so the actual thread moves may differ slightly.

It may be possible to output threads as a G76 for the older machines from QTurn but again, waht you design and what actually happens on the machine may differ slightly.
QTurn used a single pass thread so that it had full control of the threading cycle...lead in angle, number of passes, spring passes etc.. Which was not possible to control with the older G76 cycles.

Post Reply