Hello,
I am just starting to play with the Tormach mill and am encountering some problems. I've had some limited experience with desktop CNC lathes, and considerable experience with a ShopBot router, however, I am relatively new to the Tormach, but I hope to learn a lot about it over the summer.

I've been using our Partwizard software to import AutoCAD dxf files and than am converting them to g-code using the ShopBot control software. Though the software has worked quite well for us on the CNC router in our lab (working with wood and composites) I suspect I am going into a totally new area when I start cutting steel. I am basically getting the shapes that I want; however, my cuts are somewhat rough where the cutting tool is plunging into the workpiece, and there is often a gouge in the side of the part where the cutter enters. The machine seems to cut fine during the profile passes; however, there is a lot of noise when the cutting tool plunges into the workpiece. With a HSS 1/4" two flute cutter I am running the machine at about 3500 rpm and am using a feed rate of 6 ipm with a .010 doc.

I realize that my choice of software is probably not the best, but is there anything I can do to improve my surface finish? I do have access to Mastercam software, but I have not had time to learn it enough to use it yet, though that will definitely be in the near future I hope. Any information would be appreciated.

Alex Johnson

Alex, I am hardly the expert on CAM software in general, but the ideal situation on a contour or pocket is to have an arc leadin and leadout. That way, the cutter approaches the actual cutting path in a tangent and there is no discontinuity on the contour. The next best thing is to have a ramped leadin, where the cutter is following the cutting path but gradually ramping down to the cutting depth. Some software can combine the two to have a helical leadin. Plunging to depth is the worst, because the cutter deflection will be in different directions during the plunge and subsequent movement along the contour.

Your RPM and feedrate are both almost 3 times the numbers Machinist Mate (the software I use to determine the two since I don't have the "feel" for them) recommends for your cutter and material. In the absence of more sophisticated leadins, you might try just going to 1400rpm and 2.4 ipm and see what that does to the surface finish.

Randy

... and set the plunge rate to half the horizontal feed rate (1.2 IPM using Randy's numbers). You could also try roughing about .015" outside of your desired area, then taking a finish pass to clean it up if your software will let you. Carbide endmills and coolant will help tremendously, too.

Feed and Speeds will take a while to sink in, but Machinist's Mate is worth the little lunch money it costs. In fact, everything got a little easier once I started taking Randy's advice...

Regards,

- Just Gary

Feed and Speeds will take a while to sink in, but Machinist's Mate is worth the little lunch money it costs. In fact, everything got a little easier once I started taking Randy's advice...

- Just Gary

I need to look into that software, Randy saved me from buying a lot of end mills to experiment with on a job I did this week, his numbers worked the first try. For your numbers and process I would slow way down, somewhere around 1250 RPM, 2.5 IPM, .080" DOC, 40% stepover. Plunging straight into steel with a 2 flute HSS is scary, try ramping or slowing down to 1 IPM while doing it, make sure all your endmills are center cutting.

What randy said that is, 1200 rpm or so perhaps less, slow feed and flood on would be my choice. I would also choose a different endmill, two flute in steel has a lot of deflection, try a 3/8 carbide four flute maybe. Definitely need a finish pass and definitely need to ramp down instead of plunge down. Surprised you did not break an endmill that way.... good luck...peace

I agree with everything written here so far. To improve your project performance, you might want to take a deeper cut, though. If I understand the original post correctly, you are cutting only 0.01" deep. The Tormach can do way more. I would take at least 0.1 for the depth (with a 1/4 or, better, 3/8 four flute carbide, and with the cutter speed and feed rates already reported.)
Stephan

Hello,
I am just starting to play with the Tormach mill and am encountering some problems. I've had some limited experience with desktop CNC lathes, and considerable experience with a ShopBot router, however, I am relatively new to the Tormach, but I hope to learn a lot about it over the summer.

I've been using our Partwizard software to import AutoCAD dxf files and than am converting them to g-code using the ShopBot control software. Though the software has worked quite well for us on the CNC router in our lab (working with wood and composites) I suspect I am going into a totally new area when I start cutting steel. I am basically getting the shapes that I want; however, my cuts are somewhat rough where the cutting tool is plunging into the workpiece, and there is often a gouge in the side of the part where the cutter enters. The machine seems to cut fine during the profile passes; however, there is a lot of noise when the cutting tool plunges into the workpiece. With a HSS 1/4" two flute cutter I am running the machine at about 3500 rpm and am using a feed rate of 6 ipm with a .010 doc.

I realize that my choice of software is probably not the best, but is there anything I can do to improve my surface finish? I do have access to Mastercam software, but I have not had time to learn it enough to use it yet, though that will definitely be in the near future I hope. Any information would be appreciated.

Alex Johnson

when you plunge into the workpiece the tool and to a lessar extent the machine flex, and the tool will drift off to one side or another. going slower can reduce flex and drift, but ideally you should simply not plunge at your finished surface. move inward .01" or so and then take a finish pass at the end.

the same applies to ending the cut. dont just stop the tool and pull up. arc the tool off the wall a few thousands, then retract.

so its basically down to programing around the flex of the tool and machine.

im just learning all this stuff too, and thats one of the things i figured out right away after getting that type of tool entry mark on some pockets.

Thanks for the information. I will try again tomorrow using the suggestions. I have been using a flood coolant when I'm doing the cut. I don't have any carbide end mills at the moment, but I'll be ordering some shortly. I am also starting to work with Mastercam X3 and hope to be able to use this with the machine shortly which should open up some possibilites.

I'll report back when I get a chance. Thanks again.

Alex,

Again, it is probably not a CAM software issue.

The G-Code that the SW spids out is dependent on the machine and the respective postprocessor in the CAM solution. You cannot run a G-Code on a Tormach that was meant for a 50hp CAT50 spindle.


Benji

I tried it again today and had better results. I dropped the spindle speed down to 1300 and was using a .100 doc with a 2 flute carbide 1/4" end mill. My feed rate was 2 ipm and I was flooding the cut with coolant. I'm planning on trying some different cuts with it tomorrow, does it sound like I'm on track? I definitely have a lot to learn, but this is a fun machine.

Alex Johnson

Get a 4-flute carbide EM for steel!

Alex-

You need to get some understanding on how to set your speeds and feeds for various materials and cutter types. One way is to use one of the PC or online based speed/feed calculators. I use the rules of thumb below to get me close, and dial in from there on how the machine is responding.

Figuring your SFM (Surface Feet/Minute, which will determine your RPM)

SFM with HSS endmills
Stainless Steel 40
Mild Steel 100
Brass 300
Aluminum 400

With carbide endmills, multiply those settings by 3 as a starting point, so:
SFM with Carbide Endmills
Stainless Steel 120
Mild Steel 300
Brass 900
Aluminum 1200

Then:

RPM = 4 x SFM/Diameter

Now to find your feed, first calculate your chip load. A reasonable starting point for the chip load is to divide your endmill diameter by 200.

Chip Load = Diameter/200

Then to calculate your Feed Rate:

Feed Rate= RPM x Num of Teeth x Chip Load

So with your 1/4" HSS endmill in steel, your RPM should be:

RPM = 4 x 100/.25 = 1600

Your feedrate should be:

Feed Rate = 1600 x 2 x .25/200 = 4 ipm

This a starting point, I usually crank down a little from these recommended settings to see how the machine responds.

However in your last post you stated that you changed to a carbide endmill. You should recalculate the feed and speed for that endmill. Carbide endmills don't last long if they are underfed, which is what you are doing with the last feed and speed you mentioned.

As the other poster mentioned, a 4 flute endmill would be better for steel. In particular, I find the "Hanita" style variable flute carbide ones work really well on Tormach and BP sized machines. I get mine from www.maritool.com and www.lakeshorecarbide.com .

As far as your maximum depth of cut, on smaller machines this is often determined by the available spindle HP you have. However if the machine is up to it, I use the following guidelines for max radial and axial cut (borrowed from Stan Dorfeld):

Slotting: Cut Depths
6061 Aluminum, Brass - 1/2 endmill diameter
7075 Aluminum - 40% endmill diameter
Mild Steel - 30-35% endmill diameter
Stainless Steel - 25% endmill diameter

Rough Profiling Tool Overlap: 70% endmill diameter or less
Finish Profiling Tool Overlap: 3% endmill diameter

Good luck-

Paul T.