Threading

More
01 Sep 2013 21:07 #38362 by two4tom
Threading was created by two4tom
Hi,

I've been running my lathe for a awhile and I wanted to try out threading. I have been messing around trying to make a male 27mmx1.50 .3150" long thread and have failed every time. I'm just not understanding the process I think. Any help would be awesome.

Tom :S

Please Log in or Create an account to join the conversation.

More
01 Sep 2013 21:43 #38363 by ArcEye
Replied by ArcEye on topic Threading
Hi

What is it that messes up?

Are you using G76?

regards

Please Log in or Create an account to join the conversation.

More
01 Sep 2013 21:54 #38364 by two4tom
Replied by two4tom on topic Threading
Yes I am using g76. First I noticed it is wanting to cut ID instead of OD.

Please Log in or Create an account to join the conversation.

More
01 Sep 2013 22:24 #38366 by ArcEye
Replied by ArcEye on topic Threading

First I noticed it is wanting to cut ID instead of OD.


Not unless you use positive numbers where there should be negative ones and vice - versa

This is a template I used to use for cutting threads, now I use something similar in ngcgui
The actual program is to cut a 1.5mm pitch thread for a ER32 collet closing nut.

It is metric, so you will have to convert to imperial, but hopefully may get you on course.
(Threading with G76 P[itch]- Z[FinalExtent] I[ThreadPeakOffset - normally 0, neg for external]- J[FirstCutDepth - positive offset]-)
(                   R[DepthDegression 1.0 is constant depth 2.0 is constant area 1-2 depth decreases & area increases 2> area decreases]-)
(                   K[FullThreadDepth positive offset beyond I for root of thread]- Q[CompoundSlideAngle eg 29.5] )
(                   H[SpringPasses at full thread depth] E[TaperAmount in units - normally 0] L[Taper- L0 None L1 entry L2 Exit L3 Both] )

#<_Diameter>=40
#<_Z_LeadIn>=15
#<_Pitch>=1.5
#<_Z_Finish>=-15
#<_PeakOffset>=-0.2
#<_First_Cut_Depth>=0.01
#<_Depth_Regression>=1.0
#<_ThreadDepth>=1.5
#<_CompoundSlideAngle>=0
#<_Spring_Passes>=2
#<_TaperAmount>=0
#<_TaperType>=0

G18 G21 G40 G49 G54 G80 G95
G90 G7
F1.5 S300
M3
G4 P10
M7  

        (GO TO OS DIA AND Z LEAD IN )
G0 X#<_Diameter> Z#<_Z_LeadIn>
G76 P#<_Pitch> Z#<_Z_Finish> I#<_PeakOffset> J#<_First_Cut_Depth> R#<_Depth_Regression> K#<_ThreadDepth> Q#<_CompoundSlideAngle> H#<_Spring_Passes> L#<_TaperType>
G00 X45

M9
M5
G28
M30

I don't have a toolpost (ATC on slant bed lathe) so I cut threads with the tool at 90deg to the workpiece and take smaller bites to try to get a good finish

I usually lubricate by hand with neat cutting oil and because it is a slant bed the tool is upside down, which helps no end with swarf clearance.

See how you get on.

regards
The following user(s) said Thank You: two4tom

Please Log in or Create an account to join the conversation.

More
02 Sep 2013 01:13 #38376 by BigJohnT
Replied by BigJohnT on topic Threading
Is there some part of this section that is not clear?

linuxcnc.org/docs/html/gcode/gcode.html#...G76-Threading-Canned

JT

Please Log in or Create an account to join the conversation.

More
07 Sep 2013 18:03 #38531 by two4tom
Replied by two4tom on topic Threading
Hi Thanks for the help.

I have do not had a lot of time during the week to play but I did cut threads. I'm using G76 for it and I was wondering is it normal for the program to start threading at the head of the bolt to thread and work its way back towed z+? I ask this is because I made cut from Z+ to Z- which worked but at the end of the cycle it wants to go to home position whens its at Z- .5 which mean if it goes home it will wipe out the part when angles out. I hope I'm not confusing you to much.

Please Log in or Create an account to join the conversation.

More
07 Sep 2013 19:03 #38533 by ArcEye
Replied by ArcEye on topic Threading
Hi

The code was just an example, you need to adapt to suit your work.

After the threading the next command is G00 X45
which in that example will take it outside the thread diameter by some 5 mm, so it should not damage anything

If you just want to stop, remove the G28 and it will not return to home

I'm using G76 for it and I was wondering is it normal for the program to start threading at the head of the bolt to thread and work its way back towed z+?


Normally start at Z+ and work to Z-, because you need a lead in, there might be instances where the other way around was required but not often.

regards

Please Log in or Create an account to join the conversation.

More
30 Sep 2013 07:18 #39374 by two4tom
Replied by two4tom on topic Threading
I've been making some 3/8-16 threads there coming out mint. But for the life of me I cant figure out how stop this from going the wrong way at the end of the program. I had to adjust it so it doesn't crash the bit and the part. I included some pics.

Hi

The code was just an example, you need to adapt to suit your work.

After the threading the next command is G00 X45
which in that example will take it outside the thread diameter by some 5 mm, so it should not damage anything

If you just want to stop, remove the G28 and it will not return to home

I'm using G76 for it and I was wondering is it normal for the program to start threading at the head of the bolt to thread and work its way back towed z+?


Normally start at Z+ and work to Z-, because you need a lead in, there might be instances where the other way around was required but not often.

regards

Attachments:

Please Log in or Create an account to join the conversation.

More
30 Sep 2013 14:12 #39380 by ArcEye
Replied by ArcEye on topic Threading
Hi

As you are using someone elses ngcgui file to do this, rather than my code posted earlier, will need to see the g76.ngc file and any post amble file if used.

The plot makes it look as though you have a front tool lathe but are returning to a position behind and above the workpiece ( slant bed lathe home?! ) and cutting through the workpiece.

Are you using gang tooling and homing behind the Z axis line or something like that?

Just need to remove the command that is causing that move, G28 or G53 X0 Z0 probably

regards

Please Log in or Create an account to join the conversation.

More
22 Nov 2013 08:49 #41101 by naz
Replied by naz on topic Threading
Hello, I've been trying to use a ngcgui routine to do some threading and was getting some issues at the end of the threading and was wondering if anyone had a idea of what would be causing the threads to be uneven at the end of the threading. I've attached a photo and pasting the ngcgui code we are using.

Thanks,

-Michael Nazaroff

g17 (xy plane)
g20 (inches)
g40 (cancel cutter radius compensation)
g49 (cancel tool lengthoffset)
g90 (absolute distance mode)
g94 (units/min feedrate)
g54 (Coordinate system 1 default)
#<tol> = 0.001
g64 p#<tol> (path control stop)
(ngcgui: call subroutine file: ../../nc_files/g76.ngc)
(ngcgui: positional parameters:)
( #1 = tool = 2)
( #2 = rpm = 800)
( #3 = diameter = .505)
( #4 = tpi = 13)
( #5 = inital_depth = 0.005)
( #6 = thread_depth = 0.050)
( #7 = spring_pass = 1)
( #8 = z_start = 0.100)
( #9 = z_end = -1)
( #10 = x_offset = .405)
( #11 = q_angle = 29.5)
( #12 = taper = 0)
( #13 = coolant = 8)
o<g76> call [2][800][.505][13][0.005][0.050][1][0.100][-1][.405][29.5][0][8]
(ngcgui: m2 line added) m2 (g54 activated)



subroutine code:

(info: G76 threading cycle)
o<g76> sub
#<tool> = #1 (= 7 Tool)
#<rpm> = #2 (= 250 RPM)
#<diameter> = #3 (Diameter)
#<tpi> = #4 (TPI)
#<inital_depth> = #5 (= 0.005 Inital Depth)
#<thread_depth> = #6 (= 0.045 Thread Depth)
#<spring_pass> = #7 (Spring Passes)
#<z_start> = #8 (= 0.100 Z Start)
#<z_end> = #9 (Z End)
#<x_offset> = #10 (= 0.025 X Offset)
#<q_angle> = #11 (= 29.5 Combine Angle)
#<taper> = #12 (= 0 Taper 0=none 2=exit)
#<coolant> = #13 (= 8 Coolant 8 On 9 Off)

#<pitch> = [1/#<tpi>]

G7 G18 G20 G40 G49 G97
T#<tool> M6 G43
M#<coolant>
S#<rpm> M3
G0 Z#<z_start> X[#<diameter> + #<x_offset>]
G76 P#<pitch> Z#<z_end> I-#<x_offset> J#<inital_depth> K#<thread_depth> Q#<q_angle> L#<taper> E#<thread_depth> H#<spring_pass>
M5 M9
G0 Z.5
G0 X0 Z0
G49
o<g76> endsub
Attachments:

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.125 seconds
Powered by Kunena Forum