General machining question

I'm running a BP Series II Interact 4 and was milling some hot rolled steel bars. I had to cut a 1.1880 deep channel, .333 wide and was using a .025 offset cutting saw with carbide ends. I had the 1.5 X 1.5 steel jigged up and was milling the channel at a 150 RPM's at a 8 feed rate and taking a 0.0250 depth of cut. the problem was that it took almost 2.5 hrs of milling time to cut to the depth. I tried running at higher RPM's (300) and a 14 feed rate but this burned the blade. Not having much experience working with steel I was hoping that I could get some advice as to the proper speed and feed rates to get a faster work time. I went thru 3 cutter blades to cut just 8 units. the cutter blades were 5 inch diameter.

thanks in advance for the help.

ben

Quote:

---

Originally Posted by bherr

I'm running a BP Series II Interact 4 and was milling some hot rolled steel bars. I had to cut a 1.1880 deep channel, .333 wide and was using a .025 offset cutting saw with carbide ends. I had the 1.5 X 1.5 steel jigged up and was milling the channel at a 150 RPM's at a 8 feed rate and taking a 0.0250 depth of cut. the problem was that it took almost 2.5 hrs of milling time to cut to the depth. I tried running at higher RPM's (300) and a 14 feed rate but this burned the blade. Not having much experience working with steel I was hoping that I could get some advice as to the proper speed and feed rates to get a faster work time. I went thru 3 cutter blades to cut just 8 units. the cutter blades were 5 inch diameter.

thanks in advance for the help.

ben

---

RPM should be calculated based on SFPM, which is typically 80-100 for HSS tools in mild steel, and 2-3X that for carbide tools:

RPM = 4 * SFPM / ToolDiameter(in inches)

In this case, you should've been running about 120-180 RPM, so you were OK with your initial setting.

Feedrate is based on RPM, chipload per tooth, and number of teeth:

Feedrate(in IPM) = RPM * #Teeth * Chipload

Chipload should really be gotten from the tool manufacturer, but if in doubt, figure 0.001-0.002"/tooth for all but small cutters (under 1/8" or so). So, if your saw had, say, 32 teeth, you'd want to run about 5 IPM.

Depth of cut can be set to whatever you can get away with, limited by spindle power, machine rigidity, and cooling. G too deep, and the spindle will slow down, and/or surface finish will deteriorate, and/or the tool will start to heat up. If any of these happen, back off on depth, or feedrate. But, it's best to find a feedrate that works well, then set depth to what the machine will tolerate.

So, overall, your RPM was probably OK, feedrate perhaps a bit high, and depth of cut probably low, unless you were running with no, or inadequate, coolant. Coolant is critical for something like this.

Regards,
Ray L.

Why did you not use a 5/16" end mill?

Quote:

---

Originally Posted by HimyKabibble

RPM should be calculated based on SFPM, which is typically 80-100 for HSS tools in mild steel, and 2-3X that for carbide tools:

RPM = 4 * SFPM / ToolDiameter(in inches)

In this case, you should've been running about 120-180 RPM, so you were OK with your initial setting.

Feedrate is based on RPM, chipload per tooth, and number of teeth:

Feedrate(in IPM) = RPM * #Teeth * Chipload

Chipload should really be gotten from the tool manufacturer, but if in doubt, figure 0.001-0.002"/tooth for all but small cutters (under 1/8" or so). So, if your saw had, say, 32 teeth, you'd want to run about 5 IPM.

Depth of cut can be set to whatever you can get away with, limited by spindle power, machine rigidity, and cooling. G too deep, and the spindle will slow down, and/or surface finish will deteriorate, and/or the tool will start to heat up. If any of these happen, back off on depth, or feedrate. But, it's best to find a feedrate that works well, then set depth to what the machine will tolerate.

So, overall, your RPM was probably OK, feedrate perhaps a bit high, and depth of cut probably low, unless you were running with no, or inadequate, coolant. Coolant is critical for something like this.

Regards,
Ray L.

---

Thanks much Ray, Great info.

ben

Quote:

---

Originally Posted by Geof

Why did you not use a 5/16" end mill?

---

I actually tried the 5/16 end mill, but had trouble holding the tolerances once the end mill got down below .5. started going out of tolerance.

ben

Quote:

---

Originally Posted by bherr

I actually tried the 5/16 end mill, but had trouble holding the tolerances once the end mill got down below .5. started going out of tolerance.

ben

---

When cutting a slot, you need to use a smaller endmill, cut a slot down the center, then come back and do the sides. With a small endmill, and a deep slot, you need to take several light finish passes, to avoid tool flex. For these light passes, increase RPM about 30%, and reduce feed by 30-50%, for better surface finish.

Regards,
Ray L.