Need Help!- G CODEfor knurling!

[atlantic23]

hi, everyone ,can some one please help me with the code for knurling i have never done it and its 1.75 diameter steel , i have been working in cnc machining for a cople of years but never had to do any knurling so iam concernd about regular feeds and speeds what rpm an what feed i should use, on X and what on Y , thankyou for your help ,any help at all is greatly appreciated .

[g-codeguy]

There is no G-code for knurling that I know of. We don't knurl very often, and my results aren't the best, so I will let others give you instructions. I can tell you that the OD size is rather critical. And that the turned diameter depends on the pitch of the knurl.

[paul gibson]

What type of steel? 1018 or 4340? What type of knurl tool? Bump Knurl?
Scissor Knurl? Boxed Knurl? What application of knurl? To prep for a press operation, for a cosmetic, for a gripping surface. Is it called out for a "Knurl" or is it called out by a specific pitch of knurl. All the above would factor into what programming code and sequence you need.

[bobo17]

wonder if you could use a 45 deg tool and basic g1 to do a thread like procedure rt. to left then lt to right. ?

[Trent Steel]

There are no canned cycles for knurling. It's just a G01 like OD turning.

Speed should be slow, and feed should be .008-.012 IPR. Exact speed will depend on how much the workpiece is hanging out the chuck, whether you got tailstock support, etc.

Do a G1 to X0. Then Z minus to the final location. Then retract. All at the same speed.

[straggleweed]

i do this every day i use a dorian tool I'm not sure on the specifics tho but it has replaceable wheels.

the most important thing for tool life and finish is that the wheels are centered on the part, my wheels fail fast if its not perfectly centered.

its not like a regular turning tool where you can set the tool to any diameter, each new diameter has to have a new tool setting in X. due to the spacing of the wheels.

i knurl 4340 pre-hard which comes in at about 32-36rc and if the wheels are centered they will last a long time, as in several hundred parts.

first thing is to finish your part to the required size and touch off the tool to that. The small touch off marks will go away as soon as you run the knurl across it. I always touch off that size and then program the tool to run .01 under that size. If my final turned diameter was X1.75 i would program X1.74, the tool came with a chart for feeds and speeds in my material i run 116sfm and .012 feed. this has given me great results. and yes its a simple G01 move, nothing special.

the way i do it is start out in front of the part and feed across it then rapid off straight up. One of my friends suggests to stop the spindle and feed down on to the part in IPM then start the spindle and go back to IPR but ive never tryed this method since ive have good success with the previous one.

Its gonna be a noisy operation and its not gonna be any normal noise that your use to so be prepared and dont be scared the first time you do it, its really simple.

Another thing when i set Z i set it to where the wheels engage the part, but there is another half inch of tool holder out in front of that so you have to take that into account durring your set up, make sure your part is sticking out far enough so get enough knurl and you keep the front of the tool out of the jaws.

[dcoupar]

Here's an example of a working knurling program for a Doosan P240. The knurled diameter is not at the end of the part, that's why the Z-1.665 start point.

N40(T08 = STR. KNURLING TOOL 12 PITCH)
G30U0W0
T0808
G00G97G99S50M03
(KNURL)
X0.986Z-1.665M08
X0.786
G01X0.686F0.015
Z-2.737
X0.786
G97M09
G00G30U0W0
M01