Need Help!- Milling 4140 at high removal rate

[kz1670]

I am looking to speed up milling a part out of preheat treated 4140. I have gone back to 1/2 dia coated solid carbide end mills after breaking a few insert style, and slower speeds and feeds. About 80-85% of the material is removed to make this part. Maybe I should take less of a cut at a higher rate. Looking for some experience here. Suggestions about tooling, depth of cut,feeds and speeds, wet or dry etc. would be appreciated.

[dertsap]

hanita varimills eat thru 4140 incredibly well , depth of cut can usually be what ever the tool dia is ,and many times it will handle that depth at full engagement ,
if you follow manufact. specs you should get exceptional results

[kz1670]

Thanks, I will look into the tooling.

[HuFlungDung]

Tools get a lot of blame, but its not always their fault

Don't overlook the quality of the toolpath. If you've got the tool engagement varying between 50 to 100% engagement when you really want 50% continuous, then the 100% represents cutter and possible machine/workpiece overload conditions. Most often, we have had to settle for mediocre cutting so that the tool can hack the overloads in the corners.

OneCNC XR3 has new high speed machining strategies which firmly limit cutter engagement and allow you to use high DOC without the ever-present danger of the tool wandering into overloaded conditions in the corners.

This is brand new technology that has come out since XR3 has been released. I'm excited about it, and the word is only beginning to get around. OneCNC's high speed toolpaths represent a radical departure from the 'offset curves' method of toolpathing that is commonly used in many cam systems.

One advantage of high DOC, constant engagement, is that while more of the flute of the endmill gets used in the cut (more material removed per tool dollar spent), that additional length of helix engagement has a better chance of keeping the tool cutting while the next flute comes into play, and this reduces vibration and tool shock. The cutter engagement can then be tailored for the available machine horsepower or whatever the tool is capable of hacking. It looks like monster cutting at first, but the difference is that the tool doesn't go crunch and bang in the corners

Now I don't know if you're shopping for software at this time, but I thought you might be interested to know that there is something available that is no longer just run of the mill toolpaths, and its not time wasting like trochoidal paths. If you've got a lot of these parts to do, it might be worth your while to bug the guys at OneCNC to get a sample toolpath sent for you to try out. Some of us users are even willing to give away a freebie once in a while

[kz1670]

Thanks, you bring up some good points. I do have the end mill taking off more than it should in one area, the program does need refinement. I was wondering if taking less off at a higher rate is the way to approach this.
.

[5axisguy]

While again I agree with HuFlung depending on your machine capabilities, I prefer the "high speed" method. When I rough on the 5axis machine, (keep in mind this is more of a dainty machine) I use a Hitachi high feed insert tool, for example in 4140 I would run a 25mm dia. tool at about 2300rpm's with a .025 step down with a .700 stepover at around 250 in per min. This method is best for 3d contours because the steps are kept to a minimum for the remaining toolpaths, while I use the other method for harder material, only thing is then on a 3d shape you have huge scallops to deal with later.

[kz1670]

My CNC milling experience has always been on older machines, cutting in a conventional manner. I have never tried cutting in a high speed manner, nor have I talked to any one as to how this is done (example wise). I appreciate all this input.
I dont even know If my machine is capable of doing so. It has a 5HP constant load spindle,capable of 7000 rpm.
I believe the one thing I have going for me is that it is all straight 2D profiling work.

[HuFlungDung]

Originally Posted by 5axisguy While again I agree with HuFlung depending on your machine capabilities, I prefer the "high speed" method. When I rough on the 5axis machine, (keep in mind this is more of a dainty machine) I use a Hitachi high feed insert tool, for example in 4140 I would run a 25mm dia. tool at about 2300rpm's with a .025 step down with a .700 stepover at around 250 in per min. This method is best for 3d contours because the steps are kept to a minimum for the remaining toolpaths, while I use the other method for harder material, only thing is then on a 3d shape you have huge scallops to deal with later.

Since you mentioned the issue of huge stepdown staircase, OneCNC XR3 has also taken this into account and has automatic step reduction applied to any slope that needs it, so you can use a productive depth of cut all over and then the tool will quickly go just where it needs to, to reduce step down depth to your specification for the prefinish state you require. I tell you, its crazy the amount of thought and technology that they put into their high speed toolpaths

High speed toolpaths could as easily be called high volume metal removal. I don't think the paths require ultra feed rates to prove their increased metal removal compared to traditional Z level toolpaths. OneCNC's technical method means that lower horsepower machines can still utilize a greater fraction of their available horsepower for a greater percentage of the actual cutting time, because the toolpaths have eliminated the intermittent tool overloading that traditional toolpaths create. But you have to be determined to push your machine a bit more than you might be used to doing. I don't mean recklessly setting tool parameters, but you should be able to tweak a fair bit more metal removal per minute.

OneCNC's highspeed toolpaths are also somewhat rounded and curvaceous where required. This helps to smooth out high feedrate machine motion. Also, when the tool gets to an area where it loops around to widen a slot, the non-cutting portion of the loop is done at a user set "high feedrate", whatever you think your machine can handle. If the tool must travel a longer distance between different part features (while roughing one level), then the toolpaths curve up in Z just before the rapid retraction, then feed back down and curve back into the cut on the XY plane. This further promotes smooth machine motion, and looks very fluid when you witness it.

You might guess that the programs grow somewhat larger. There are some interpolated moves that add to program length, but program length can be a concern on an older machine with limited memory. However, fewer Z level repetitions can go a long ways toward reducing program length, too.

This is where OneCNC is also designed for state of the art controllers that can handle large programs and process a lot of blocks quickly. I like having 16 megs on my Haas, and never having to worry about program lengths

[kz1670]

It sounds like the toolpath is key to proper tool life and making this work. As long as you have the proper control on the machine end.