[Potatohead908]

I'm trying to wrap my head around all the feed's and speeds terminology. I have a 3/8" OSG (PN# 5350500) 2 flute, HSS end mill. Looking at their site it seems I am looking at running a .0375 step over at 23 IPM but that is at a depth of 1.5 x the diameter of the tool. If I am doing a pocket from scratch I will be ramping down about .04 inches, roughing out the pocket, ramp down another .04 inches and so on. OR do I just spiral plunge the whole 1.5 x the diameter of the tool which equals .5625 and rough the pocket? The second option would be BADA** since I've never done anything that aggressive (on purpose).

I am using a CNCed G0704 with a stock 1100 watt motor.

[Potatohead908]

Did I not word my first post well? Does it not make sense?

[mmoe]

What spindle RPM?

I've 1.5 times the diameter is only a little over half an inch. You'll need coolant with the HSS bit, but otherwise I don't see any reason you couldn't give that a shot. I usually use Carbide and have never had much problem doing a half inch adaptive roughing pass with it, even without coolant. If you're only engaging 10% of the cutter diameter, I'm guessing it must be an adaptive strategy (trochoidal/HSM) If not, you'd be better off going old school and taking shallow passes with HSS.

[Fastest1]

Stock 1100 watt motor? Stock is 750 IIRC.

[Potatohead908]

Stock 1100 watt motor? Stock is 750 IIRC.

I just went and looked. For some reason I thought that there was something on the motor or cover that said 1100 watts but I can't find it. The face plate on the mill says 750 so I was mistaken. Sorry about that.

[Potatohead908]

What spindle RPM?

I've 1.5 times the diameter is only a little over half an inch. You'll need coolant with the HSS bit, but otherwise I don't see any reason you couldn't give that a shot. I usually use Carbide and have never had much problem doing a half inch adaptive roughing pass with it, even without coolant. If you're only engaging 10% of the cutter diameter, I'm guessing it must be an adaptive strategy (trochoidal/HSM) If not, you'd be better off going old school and taking shallow passes with HSS.

mmoe, On the OSG site it shows slotting for my end mill and that is all. I have searched the pages this morning and can't find the page I got the numbers from for just HSS side milling. Not a fan of their site. I downloaded FSWizard lite last night. FSWizard is showing .520 DOC, .038 WOC, 3150RPM at 11.6 in/min.

[Potatohead908]

Oh and I don't have flood coolant yet. Planning on having that setup in the next two weeks with an enclosure. I have a spray bottle of WD-40 and a 60 gallon air compressor for now, along with aluminum chips in every crack and corner! I'm going to air cut first, then wood and then after that try a few different models so that I prove that I have a bit of a handle on it. Build the enclosure, coolant system, upgraded stand and chip collection over the next few weeks then go for more aluminum cuts. I will probably try one or two using aluminum with the air and WD-40 between now and then unless others think I will destroy my end mill trying that....

[Potatohead908]

I'm trying to wrap my head around all the feed's and speeds terminology. I have a 3/8" OSG (PN# 5350500) 2 flute, HSS end mill. Looking at their site it seems I am looking at running a .0375 step over at 23 IPM but that is at a depth of 1.5 x the diameter of the tool. If I am doing a pocket from scratch I will be ramping down about .04 inches, roughing out the pocket, ramp down another .04 inches and so on. OR do I just spiral plunge the whole 1.5 x the diameter of the tool which equals .5625 and rough the pocket? The second option would be BADA** since I've never done anything that aggressive (on purpose).

I am using a CNCed G0704 with a stock 1100 watt motor.

For the record....My machine is not ready to make option two work. I had the tts tool holder pull out. I have added some more compression to the Belleville washers and reduced my engagement to .0175 WOC, 0.56 DOC, 2500 RPM and 25 IPM. Will let you know if that doesn't work either.

Ok this cut did work. Not the best finish however the end mill is hammered and to make it worse it started life out in one of those 12 pc. cheapy sets.

[mmoe]

Oh and I don't have flood coolant yet. Planning on having that setup in the next two weeks with an enclosure. I have a spray bottle of WD-40 and a 60 gallon air compressor for now, along with aluminum chips in every crack and corner! I'm going to air cut first, then wood and then after that try a few different models so that I prove that I have a bit of a handle on it. Build the enclosure, coolant system, upgraded stand and chip collection over the next few weeks then go for more aluminum cuts. I will probably try one or two using aluminum with the air and WD-40 between now and then unless others think I will destroy my end mill trying that....

If it were me, I'd stick with carbide until you can get more coolant on there. HSS is sharp, but not for long if it gets hot. If set to the correct feed/speeds, carbide can take a lot more abuse. If you mist WD-40 onto the part with a good carbide bit, you'll be able to get a nice finish out of it. Don't go cheap on carbide bits, they are usually not very sharp if you do. A high quality carbide bit will last and cuts nearly the same as HSS anyways.

[Potatohead908]

If it were me, I'd stick with carbide until you can get more coolant on there. HSS is sharp, but not for long if it gets hot. If set to the correct feed/speeds, carbide can take a lot more abuse. If you mist WD-40 onto the part with a good carbide bit, you'll be able to get a nice finish out of it. Don't go cheap on carbide bits, they are usually not very sharp if you do. A high quality carbide bit will last and cuts nearly the same as HSS anyways.

This is good information mmoe. Thank you. I have one 3/8" carbide end mill. It is from Enco and it's an Atrax. Feels sharp as all heck but I think they are a cheaper verity...? I'm hesitant to use anything good right now as I am still learning and the sting of loosing my OSG end mill yesterday is still fresh. It probably had 5 inches cut time Oh on the upside Enco is having 20% off, free shipping and no minimum today and tomorrow so I will be purchasing some more end mills! Atrax OK?

[mmoe]

I really don't know any brand names, crazy as that may sound (at least for machine tool bits, I use Vortex for router bits/plastics). I just call up the tool supply house and tell the guy what I'm doing. He then tells me what should work best. Usually he's right on, sometimes he's off. In the case of the latter, it's usually a very special application where he's never had anyone do exactly that before. I couldn't even tell you what brands he gives me as I just trust that whatever he sells me is going to be plenty good. If you have a local tool supplier like that, they are often not much more expensive but provide a lot of knowledge. Here's who I use here:

Cutting Tool Control, Inc

[SCzEngrgGroup]

If it were me, I'd stick with carbide until you can get more coolant on there. HSS is sharp, but not for long if it gets hot. If set to the correct feed/speeds, carbide can take a lot more abuse. If you mist WD-40 onto the part with a good carbide bit, you'll be able to get a nice finish out of it. Don't go cheap on carbide bits, they are usually not very sharp if you do. A high quality carbide bit will last and cuts nearly the same as HSS anyways.

If the tool is getting hot enough that the heat tolerance of carbide vs HSS is an issue, you're feeds and speeds are off by MILES, and you're going to get into chip welding long before you see any difference at all between HSS and carbide. A hot tool indicates too much RPM and/or too little feed for the conditions. When feeds and speeds are right, the heat is carried away by the chips, and the tool stays cool, until you get into spindle power levels far beyond what a G0704 has. As for carbide taking more abuse, carbide is generally much easier to chip and damage, even by simply re-cutting a few chips. Given the MUCH higher cost of a quality carbide tool vs a quality HSS tool (and cheap in either == JUNK), it makes little sense on smaller machines, which have neither the RPM, nor the power, nor the rigidity to get any real benefit out of carbide.

On my Novakon Torus Pro, I use HSS almost exclusively, except for smaller tools (under 1/4") where the added stiffness of carbide is beneficial. My standard roughing cut, with a $12 HSS 1/2" 2-flute, is 1/2" DOC, 0.050" WOC, 5000 RPM, 110 IPM. I can cut like that for days with the same tool. Carbide would gain me nothing, other than higher cost.

Regards,
Ray L.

[hoss2006]

This is good information mmoe. Thank you. I have one 3/8" carbide end mill. It is from Enco and it's an Atrax. Feels sharp as all heck but I think they are a cheaper verity...? I'm hesitant to use anything good right now as I am still learning and the sting of loosing my OSG end mill yesterday is still fresh. It probably had 5 inches cut time Oh on the upside Enco is having 20% off, free shipping and no minimum today and tomorrow so I will be purchasing some more end mills! Atrax OK?

I got that deal earlier today, needed a 5/16 endmill with 1 5/8 length of cut for an 80% lower, it was an american made Atrax carbide which is the way to go for stiffness with that length of cut.
Hoss

[Potatohead908]

If the tool is getting hot enough that the heat tolerance of carbide vs HSS is an issue, you're feeds and speeds are off by MILES, and you're going to get into chip welding long before you see any difference at all between HSS and carbide. A hot tool indicates too much RPM and/or too little feed for the conditions. When feeds and speeds are right, the heat is carried away by the chips, and the tool stays cool, until you get into spindle power levels far beyond what a G0704 has. As for carbide taking more abuse, carbide is generally much easier to chip and damage, even by simply re-cutting a few chips. Given the MUCH higher cost of a quality carbide tool vs a quality HSS tool (and cheap in either == JUNK), it makes little sense on smaller machines, which have neither the RPM, nor the power, nor the rigidity to get any real benefit out of carbide.

On my Novakon Torus Pro, I use HSS almost exclusively, except for smaller tools (under 1/4") where the added stiffness of carbide is beneficial. My standard roughing cut, with a $12 HSS 1/2" 2-flute, is 1/2" DOC, 0.050" WOC, 5000 RPM, 110 IPM. I can cut like that for days with the same tool. Carbide would gain me nothing, other than higher cost.

Regards,
Ray L.

I cant come close to that cut from what I can tell. Obviously I don't have 5000 rpm to work with. I hope to buy a Torus Pro this coming year but until then I have to take MUCH smaller bites. I've done some chip welding today! However I finally found a successful cut with a cheap 3/8" end mill at .0175 WOC, 0.56 DOC, 2500 RPM and 25 IPM. I have no doubt a better end mill would have would have a much better finish. Plus tweaking these numbers would also help. Also using the adaptive cutting I think I should leave some stock and do a more traditional finishing pass. With my CAM it doesn't allow me to enter any finishing information while using the adaptive milling.

I downloaded a trial version of GWizard yesterday. That helped but there is still some trial and error to work through on all this. I am learning a lot these past few days!

[Potatohead908]

When using adaptive machining protocol do you do a separate finishing pass? I'm thinking I need to for a better finish. I'm sure finding ideal feeds and speeds will improve the finish just within adaptive machining. I noticed a some deflection using just the adaptive protocol is why I ask.

[hoss2006]

When using adaptive machining protocol do you do a separate finishing pass? I'm thinking I need to for a better finish. I'm sure finding ideal feeds and speeds will improve the finish just within adaptive machining. I noticed a some deflection using just the adaptive protocol is why I ask.

I do, I check the box for multiple depths at about .200, check the box for stock to leave at .005 and let it create the toolpaths. rename the file with rough in the name. right click and duplicate it. rename the duplicate with finish, edit it and uncheck both multiple depths and stock to leave, let it create the toolpath and then you have roughing passes and a finish pass.
Hoss

[SCzEngrgGroup]

When using adaptive machining protocol do you do a separate finishing pass? I'm thinking I need to for a better finish. I'm sure finding ideal feeds and speeds will improve the finish just within adaptive machining. I noticed a some deflection using just the adaptive protocol is why I ask.

Adaptive is for roughing only, and makes no attempt to leave a nice surface, especially on side walls.

Regards,
Ray L.

[Potatohead908]

Thank you both! I will start implementing a final cleaning protocol.

[Fastest1]

And you can run that finish pass more than once, I prefer 2-3 quick finish passes just to be sure any tool deflection is taken care of as good as can be.

[Potatohead908]

And you can run that finish pass more than once, I prefer 2-3 quick finish passes just to be sure any tool deflection is taken care of as good as can be.

Thanks Fastest1. That makes sense. My CAM program makes this super easy.