[mioduz]

I always used FSwizard to calculate feeds and speeds, with a high level of success. Tormach had a sale on Gwizard and I had heard many good things, so I bought a liscense.
Ive noticed in the pas that Gwizards feeds where a bit "aggressive" for drilling operations, so much to the point where I would be runnning to slow down the feed on the machine becuase i thought i was going to ruin something.
Just got my first face mill (fairly cheap model from shars) 1.5" with 4 teeth.
I put the same info into both calculators and came up with a reasonably close RPM difference, but feed rates nearly 4x faster with GWizard.
Maybe I am doing something wrong, what does everyone on here think. I just dont want to burn up a set of inserts with bad numbers

[SCzEngrgGroup]

Personally, I much prefer HSMAdvisor, and I can't think when it's ever steered me significantly wrong. When it's numbers are slightly too aggressive, it's because of limitations in the machine. In most cases, I now take it's numbers and run with them, with little or no testing. In this case, the GWizard numbers do seem very aggressive.

Regards,
Ray L.

[GJeff]

Agreed. FSWizard is great. Their numbers seem more real world for obtaining good cuts whereas GWizard is some theoretical maximum.

[SCzEngrgGroup]

BTW - HSMAdvisor gives 600 RPM @ 6.4 IPM for that cut, which seems reasonable to me.

Regards,
Ray L.

[hjl4]

HSM Advisor all the way. It also beats FeatureCam hands down on F and S. I tried GWizard, and I too, got way nervous watching tools plunging at high feed rates. Never broke a tool with it though but just doesn't seem right.

[zero_divide]

I always used FSwizard to calculate feeds and speeds, with a high level of success. Tormach had a sale on Gwizard and I had heard many good things, so I bought a liscense.
Ive noticed in the pas that Gwizards feeds where a bit "aggressive" for drilling operations, so much to the point where I would be runnning to slow down the feed on the machine becuase i thought i was going to ruin something.
Just got my first face mill (fairly cheap model from shars) 1.5" with 4 teeth.
I put the same info into both calculators and came up with a reasonably close RPM difference, but feed rates nearly 4x faster with GWizard.
Maybe I am doing something wrong, what does everyone on here think. I just dont want to burn up a set of inserts with bad numbers

Before you press the green button do yourself a favour and download HSMAdvisor from Advanced CNC Speed And Feed Calculator - HSMAdvisor
Select "Tormach lower range" machine from the list of machines and puch the numbers for the cut you are going to take.
I didnt check, but i have a feeling yor machine may not have balls(torque) to do the cut.

[tbaker2500]

You don't show where you have the slider on Gwizard. That significantly adjusts the numbers.
I note that you have chip thinning selected on gwizard but not on fswizard. You will want it on on both for a large cut like this.
You are definately going to want to be using the low-speed belt setting, regardless.
I've never had Gwizard give me a wrong number. I trust it, and it's never let me down.
However, it's important to recognize the variety of options available to you. A roughing cut is going to be just that. A heavy cut designed for maximum material removal. Middle two positions give you light roughing cuts, which may pass for finish cuts. And left most is a really slow, light finish cut, It will give you a great finish, but take a long time.

[tmarks11]

GWizard and FSWizard are giving you too slow an rpm, probably because of the range of hardness selected for 4130. 4130 ranges in recommended sfm from 310 (HB 175-225) to 140 (HB 375-425) fpm. Are you really sure you are dealing with something that hard?

sfm*4/D = 310 *4/1.5 = 830 rpm (for HB 175-225 case)

Can't really tell what chip load FSWizard is using, but 0.007 ipt for GWizard is right-on. Of course, increasing rpm increasing the feed rate proportionately, leaving you with 23 ipm. I bet you wil be running against spindle hp in with that kind of feed rate and DOC.

ipm = 0.007 ipt * 4 teeth * 830 rpm= 23 ipm

Q = 23 *1.5*0.05= 1.725 ci/min
P = 0.56*1.11*1.725*1.25 = 1.34 hp

yep, aggressive on a 1.5 hp mill. I would try it with 12 ipm and 830 rpm. If I am wrong about hardness, the next step down would seem to be pretty close to what Ray gave you.

And all that math is why you use GWizard, FSWizard, or HSMAdvisor. Of course your results are only as good as your inputs.

FSWizard at 4 ipm? Wimpy. I am betting one of your constants you selected is wrong, because there is no way it should be giving you that slow a speed. I don't know why you are getting 168-169 fpm in both cases, that is a bit slow for carbide + 4130 in anything but the hardest HB material.

[zero_divide]

GWizard and FSWizard are giving you too slow an rpm, probably because of the range of hardness selected for 4130. 4130 ranges in recommended sfm from 310 (HB 175-225) to 140 (HB 375-425) fpm. Are you really sure you are dealing with something that hard?

sfm*4/D = 310 *4/1.5 = 830 rpm (for HB 175-225 case)

Can't really tell what chip load FSWizard is using, but 0.007 ipt for GWizard is right-on. Of course, increasing rpm increasing the feed rate proportionately, leaving you with 23 ipm. I bet you wil be running against spindle hp in with that kind of feed rate and DOC.

ipm = 0.007 ipt * 4 teeth * 830 rpm= 23 ipm

Q = 23 *1.5*0.05= 1.725 ci/min
P = 0.56*1.11*1.725*1.25 = 1.34 hp

yep, aggressive on a 1.5 hp mill. I would try it with 12 ipm and 830 rpm. If I am wrong about hardness, the next step down would seem to be pretty close to what Ray gave you.

And all that math is why you use GWizard, FSWizard, or HSMAdvisor. Of course your results are only as good as your inputs.

FSWizard at 4 ipm? Wimpy. I am betting one of your constants you selected is wrong, because there is no way it should be giving you that slow a speed. I don't know why you are getting 168-169 fpm in both cases, that is a bit slow for carbide + 4130 in anything but the hardest HB material.

Well, to be fair i have not updated my free online calc for a very long time. For my own work i use HSMAdvisor at the PC and FSWizard app for my android phone.
I am sticking 100% to the results they are giving to me.
here is what i get for 4130 steel with coated inserts and i know it works.
Only thing is you got to keep the DOC down for less than rigid/powerful machines.

[tmarks11]

Well, to be fair i have not updated my free online calc for a very long time.

Good to know. You might want to put a banner on that page directing users to your more accurate downloaded version; I would hate to think you would lose customers cause someone tried your free online version, saw results that looked iffy, and assumed your more accurate download version would give similar answers.

504 sfm seemed a bit fast (I was looking at Moltrecht "Machine Shop Practice")... you made me get up and go to the garage to get the 28th Machine Shop Handbook.

Yep, there it is, 505 sfm for coated carbide. What do you know, maybe I need to download your program (it agrees with the Handbook better than GWizard does). Although he needs to tone it down a bit to keep within his spindle power limit.


sfm*4/D = 505 *4/1.5 = 1346 rpm (for HB 175-225 case)

ipm = 0.007 ipt * 4 teeth * 1346 rpm= 38 ipm

But we already know that is over his power limit, so backsolving with 1 HP for Q and feed:
Q = 1/(0.56*1.11*1.25) = 1.287 ci/min
feed = 1.287/1.5/0.05 = 17 ipm

So 1350 rpm at 17 ipm should require 1 HP spindle speed. I would leave DOC the same and just slow the feed down (too little DOC just wears out your cutter and adds heat).

For increased insert life, the rule is to generally adjust feed, then rpm, then DOC, in that order.