Numbers for threading Stainless

Can someone give me their recommendations on setup for cutting
internal and external threads in 303 and 304 stainless? This is my
first time programming to cut threads in stainless and would just like
some pointers. I'm using an insert type threading tool with sandvik
423 carbide inserts. 3/4" tool holder. The first thread i need to cut
is 1.25-20 and I got numbers of: 580SFM for 303 and 250 SFM for 304. ,
and a .015" DOC. am i even close?
Reply to
charles
Loading thread data ...
I thread alot of stainlesss What kind of control are you using? What does DOC mean? I asume this is a lathe.1 1/4 dia. ,303 stainless 580 surface feet min. 580 x 3.82 / 1.25= 1772 rpm that seem a little fast to me i would start at about 1000 rpm. Your leed will be .05 per rev. (1.00 / 20=.050 ) To find your thread height external. multiply leed x .61343 (.05 x .61343 = .0306) This is the height of the thread per side . So (.0306 x 2=.0612 ) 1.25 - .0612= 1.1888 this will be your final thread depth for x axis. To find the depth of thread for an internal thread mutiply thread leed x .54127 If you are using a Fanuc control your threading program might look like this depending witch model of control you have.This how I woud write it for a Fanuc 21T control
O1234 S 1000 M3 T0101 GO X 1.270 Z.1 M8 G76 P010160 Q0020 R.001 G76 X 1.1888 Z- 1.00 P0306 Q0050 F.050 M30
This program will cut an external 1.25 dia. 20 threads per inch ,1 inch long.
O1234( is just the program number ) S 1000 M3 ( the S calls for spindle, 1000 is rpm , M3 turns spindle on foward M4 is reverse. T0101 (T01 turns turret to tool 1 witch is going to be our threading tool the 01 is the tool off set . GO X 1.270 Z.1 ( GO is a rapid move the threading tool will travel at full speed to X1.270 and Z.1 this will place the threading tool a little above the shaft and .1 inch in front of the shaft M8 turns coolant on M9 coolant off
The G76 is a thread cuting cycle ,on a fanuc 21t control it uses 2 lines or 2 blocks ( a block is a single line of code) It will thread in at 29 deg. 1st block or line G76 P010160 Q0020 R.001 G76 call for threading cycle P010160 the first 2 digits 01 is number of spring passes or finishing cuts ,( Its just a pass with out moving the infeed in ,you can make 0 passes or up to 99 The thrid and forth digit is the thread let off 01 so on last thread it will gradully pull out so the thread just does not stop suddanly . If your threading up to a sholder and you want the nut to go as far as it can put 00 for the second and third digits this will suddanly stop the thread just before it hits the sholder. The forth and fith digits is the angle of the thread 60 is for a 60 deg.thread or 29 for a acme thread 29 deg. Q is the depth per pass radial, Q0020 this will feed the threading tool down .002 per pass or .004 dia. R is the infeend amount for last pass it feeds straght in insted or 29 deg. it just cleans the thread up.
Second G76 line G76 X 1.1888 Z- 1.0 P0306 Q0050 F.050 G76 call up thread cycle X 1.1888 is the depth of last cut Z-1.00 The thread is 1 inch long P0306 is the thread height .0306 inchs per side. Q0050 is the first threading pass. The first pass can be cut deeper. F.05 The f is for feed how far the thread advances per revolution , in this case 20 threads per inch 1inch /20 = .050 inch.
M30 end of program stop spindle turns coolant off returns to start or program.
The G76 threading cycle may seem complicated but its a lot easyer than writing it long hand it is a very powerfull caned cycle it took only 8 blocks (lines) and feed the threading tool in at 29 deg. If i could to write this program long hand and feed the tool in at 29 deg. it would take alot or figuring and alot of lines of code. And if i wanted to feed a little deeper all i have to change just 1 number. Hope this helps .
Reply to
TLKALLAM8
very helpful.
thanks
I'm using mazatrol on a SQT 250 turning center with a fusion 640 controller. DOC= Depth of cut
Reply to
charles
What kind of control are you using? I asume this is a lathe.1 1/4 ,303 stainles 580 surface feet min. 580 x 3.82 / 1.25= 1772 rpm that seem a little fast to me i would start at about 1000 rpm and work my way up. Your leed will be .05 per rev. (1.00 / 20=.050 ) To find your thread height external. multiply leed x .61343 (.05 x .61343 = .0306) This is the height of the thread per side . So (.0306 x 2=.0612 ) 1.25 - .0612= 1.1888 this will be your final thread depth for x axis. To find the depth of thread for an internal thread mutiply thread leed x .54127 The .015 deepth or cut is a little to much I would go about .005 per pass. Also always start you threading tool at least 2 thread starts in front of your part .This will give the encoder time to find the start point and get the thread tool up to threading speed.
If you are using a Fanuc control your threading program might look like this depending witch model of control you have.This how I woud write it for a Fanuc 21T control
O1234 S 1000 M3 T0101 GO X 1.270 Z.1 M8 G76 P010160 Q0020 R.001 G76 X 1.888 Z- 1.00 P0306 Q0050 F.050 G0 Z6. M30
This program will cut an external 1.25 dia.-20 threads per inch ,1 inch long.
O1234( is just the program number ) S 1000 M3 ( the S calls for spindle, 1000 is rpm , M3 turns spindle on foward M4 is reverse. T0101 (T01 turns turret to tool 1 witch is going to be our threading tool the 01 is the tool off set . GO X 1.270 Z.1 ( GO is a rapid move the threading tool will travel at full speed to X1.270 and Z.1 this will place the threading tool a little above the shaft and .1 inch in front of the shaft M8 turns coolant on M9 coolant off
The G76 is a thread cuting cycle ,on a fanuc 21t control it uses 2 lines or 2 blocks ( a block is a single line of code) It will thread in at 29 deg. 1st block or line G76 P010160 Q0020 R.001 G76 call for threading cycle P010160 the first 2 digits 01 is number of spring passes or finishing cuts ,( Its just a pass with out moving the infeed in ,you can make 0 passes or up to 99 The thrid and forth digit is the thread let off 01 so on last thread it will gradully pull out so the thread just does not stop suddanly . If your threading up to a sholder and you want the nut to go as far as it can put 00 for the second and third digits this will suddanly stop the thread just before it hits the sholder. The forth and fith digits is the angle of the thread 60 is for a 60 deg.thread or 29 for a acme thread 29 deg. Q is the depth per pass radial, Q0020 this will feed the threading tool down .002 per pass or .004 dia. R is the infeend amount for last pass it feeds straght in insted or 29 deg. it just cleans the thread up.
Second G76 line G76 X 1.888 Z- 1.00 P0306 Q0050 F.050 G76 call up thread cycle X 1.888 is the final depth of thread Z-1.00 The thread is 1 inch long P0306 is the thread height .0306 inchs per side. Q0050 is the first threading pass. The first pass can be cut deeper. F.05 The f is for feed how far the thread advances per revolution , in this case 20 threads per inch 1inch /20 = .050 inch. G0 Z6.0 Rapid threading tool away from part 6 inchs M30 end of program stop spindle turns coolant off returns to start or program.
if you don't have a g76 cycle I can write it long hand . Hope this helps.
Reply to
TLKALLAM8
On a Mazatrol, Just use the auto function when programming. It works very well for automatically calculating depths of cut. The numbers you got for threading that grade of stainless are pretty close. You may want to change the parameter for minimum depth of last cut to .002 for stainless. Spring passes on stainless kill the insert for long production runs. Run one with 0 x offset and measure the pitch dia. Adjust offset so the next part comes out near the minimum pitch dia., and change the insert when it gets near the maximum size.
Steve Walker
Reply to
Steve Walker

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.