By jack
August 29, 2014, 3:19 am
confuse about Chip thinning and HSM
1045 STEEL, 10FLAT END MILL, 4 flutes , CARBIDE, TIN. DOC:12MM. 1: WOC=DEFAULT=4(40% STEP OVER) RPM 4263, FEED:911, MRR:43.8, TOOL LIFE:161%. 2: WOC=0.8(8% STEP OVER), CHIP THINNING CHECK，HSM check。 RPM=7858,FEED:4642, MRR:44.57(almost the same as above), TOOL LIFE: 89%(MUCH less) what do you prefer??? in condition 2, if uncheck the HSM, then you will get: RPM:4263, FEED:2518, MRR:24.18, TOOL LIFE:288%. that is almost half MRR with almost 2 times tool life of condition 1. and i think it's the same result as condition 1， because you need to mill longer time to remove the same material.
Eldar Gerfanov (Admin)
Updated by: Eldar Gerfanov (Admin)August 29, 2014, 5:55 am
Hi. Tool life is ESTIMATED based on time, not the amount of material it removes. In my testing i found out that generally tool life estimation works more or less good. There are however some quirks. Especially when it comes to HSM vs Conventional milling. Real tool life is very mich dependant on cutting speed. So, in answer to your first question, i would still use the Chip thinning method #2, but reduce the cutting speed override to maybe 80%. You will notice how tool life increases. To further optimise tool life, i would increase feed override to about 120-150% This will have modest impact on tool life, but will increase MRR. Regarding the last question. Where you switch off HSM and tool life jumps. It is because you are now using much lower cutting speed. And cutting speed is the main factor that determines the tool life. Good luck. Let me know how it goes :ernaehrung004:
jack
hi? thanks for your reply. i know reducing the cutting speed will increase the tool life. in condition 2, you need to reduce the speed to 73%, then you will get this: RPM 5736, FEED:3388, MRR:32.53, TOOL LIFE: 163%(same tool life with condition 1). compare with the condition 1, i can't not see any benefit of this(in fact it have disadvantage of less MRR). is it means HSM AND chip thinning are useless??
Eldar Gerfanov (Admin)
Formula for tool life is not perfect. In regular machining imcreased chiplpad causes tool life to decrease. In HSM machining, however, increased chiplpad actually improves the tool life. So, what you should be tying to do is increase feedrate even higher. 100% feed is very conservstive. I personally use 150% feed override. I also increase Torque Limit to 150%, so that it does not complain. Many people use feed override of 200% and up. There is almost no cealing especially with softer materials Also HSM machining productivity is very dependant on part geometry. Recommended DOC is above 2x diameters. More than 4 flutes is recommended as well. When cutting shallow features with few cuttimg edges, it may not be worth it to employ the HSM at all and go with conventionall.