16MM carbide bullnose cutter 4mm corner radius - young CNC programmer issues!

Danjones777 · Dec 5, 2019

Hi all, i am a young CNC programmer that has come across a slight issue. A feature on a part i am machining is a 25mm wide slot that is 585mm long and has a 4mm radius in either corner, the slot is to finish 8mm deep. Initially, i am using an 18mm rippa cutter. i am machining the slot to 24mm wide and 4.5mm deep, and then running the rippa cutter along the centre of the slot 7.5mm deep. this leaves two squares of materials in the corners of the slot to machine the radius with my 16mm carbide bullnose cutter with a 4mm corner radius. (please see attached photo for context). now, I've completed 10 parts and they are correct dimensionally but i have managed to chip two of my bullnose cutters. I am a relatively inexperienced programmer so I'm not sure as to what I'm doing wrong, could it be the amount of material i am trying to clean up in one go with my Bullnose cutter? or are my feeds and speeds wrong? i am running the cutter at 5000RPM and the feed 1000mm/min, the component i am machining is Aluminium. the cutters are almost £200 a pop so i don't particularly want to chip/scrap anymore.

if any more experienced heads have any guidance for me it would be much appreciated.

dandrummerman21 · Dec 5, 2019

Can you post a picture of the damaged tools?

I'd say the rpm is too high (not actually too high, it is aluminum, but I would slow it down when you have issues) and the feedrate is a bit low for the RPM.

Without seeing how it failed, I might suggest that you add another rough pass with a square endmill to make the step less. But then again, I don't think you should have this issue with aluminum.

What does the workholding look like? Rigid? How about the tool, is it stubby? long? What kind of machine? Is the machine rigid? Also, what kind of aluminum? And what is the coolant situation?

Hardplates · Dec 5, 2019

Just speculation but it sounds like something is moving around (work, tool, spindle, table...) and causing the cutter to grab a big bite and chip. It's kind of tough to chip a cutter in aluminum.....at least that has been my experience.

GENERALDISARRAY · Dec 5, 2019

200 POUNDS IS LIKE 300 YANKEE BUCKS?!!

for a 5/8 endmill?!
if you had them modified with that big CR then I think that (the sharpenin dude)is your problem

At the aerospace shop I worked before we ran 3/4 necked EMs with .19 CR wide open (10-24K) squackin and chirping climb/conv all day. They would still last forever.

Danjones777 · Dec 5, 2019

dandrummerman21 said:
Can you post a picture of the damaged tools?

I'd say the rpm is too high (not actually too high, it is aluminum, but I would slow it down when you have issues) and the feedrate is a bit low for the RPM.

Without seeing how it failed, I might suggest that you add another rough pass with a square endmill to make the step less. But then again, I don't think you should have this issue with aluminum.

What does the workholding look like? Rigid? How about the tool, is it stubby? long? What kind of machine? Is the machine rigid? Also, what kind of aluminum? And what is the coolant situation?

I will post a picture of the top first thing in the morning! Okay, I actually thought the feed rate was too fast.. what feed rate would you suggest to speed up to? Others have suggested possibly completing my slot in two steps with my CR bullnose cutter, down to 6.5mm deep and then to 8mm deep. I guess this is the same as have a smaller step as you’ve suggested really. I am holding the part with two vices, there certainly doesn’t seem to be much vibration. The machine is a 3 axis milling machine, it is rigid. Bed size is 2.6m by 1.1m. I can send photos of my machine and set-up tomorrow if this helps?

TeachMePlease · Dec 5, 2019

Hmm... 2 vices... If the depth of that slot in your image is 7.5mm, extrapolating, your plate is about 25mm thick... How long/wide is this plate that needs to be held in two vices? Is this slot feature perhaps in the area of the plate that's hanging out in space between the two vices?

It's pretty difficult to break a cutter in aluminum without extreme feedrates or just bad cutting conditions... Vibration, even small vibration that you don't see will chip a cutter though... How does the machine feel/sound during these cuts? Any weird noises? How are you evacuating chips? Air blast? Flood coolant?

Danjones777 · Dec 6, 2019

please see below comment

Danjones777 · Dec 6, 2019

please see attached picture of the damaged tools, and the part I am machining. it is extruded aluminium, I am holding on to the bottom flange with the two vices. the coolant situation isn't great.. which could be an issue I guess.

see attached picture and let me know your thoughts.

Milland · Dec 6, 2019

Does seem an odd failure for an aluminum cut. You do have a long trough, and if the coolant isn't enough to clean out the chips you may be recutting them, which even with Al is not a good thing for endmills.

If surface finish and noise during the cut (no screeching or ringing) are OK, then the likely culprit is chip recutting. Focus on coolant flushing of the chips, if you can't improve coolant flow try doing a roughing pass for both sides in a "conventional" direction, then follow with two climb cuts for finishing.

Also, do what you can to shorten the tool stickout length, a short holder will help. Those cutters can be reground, you'll save money with that over buying new. Problem may be finding a good, reliable tool regrinder in your area.

Danjones777 · Dec 6, 2019

to be fair, the coolant flow on my machine isn't great.. i'll look into ensuring this is sorted before running the next trials and hopefully this should solve the issue. i'll experiment with the conventional roughing cuts too, thanks for the feedback.

dandrummerman21 · Dec 6, 2019

Is that endmill coated with AlTiN or TiAlN? Or does it just seem like it has that coating because of the light?

If that has one of the coatings I mentioned above, that could be a part of the problem. Aluminum sticks to those coatings, which would have you welding chips to the tool and then the next revolution would snap it off while welding another chip to it.

You would be better off having an aluminum coating (like ZRN), or simply uncoated carbide (that's what I would do for this; cheaper too).

If it isn't coated and it is just the lighting that makes it look like that, Milland has a point.

If it is coated, you can probably still get through with the very expensive tools you already paid for, maybe just lower the rpm some. It would stick less with less heat generated.

FWIW in the future, a couple things you might do instead of this large expensive tool:

1: grind your own radius on a tool.
2: Instead of a large bullnose cutter with 4mm radius, you could buy an 8mm ball endmill for a lot cheaper. Use the ball endmill to finish the corners only. Hell, you could rough your current part further with an 8mm ball and use your bullnose to finish the slot to make it look pretty.
3: buy a HSS tool with radius. Its just aluminum, you can go pretty fast in aluminum with HSS too.

Danjones777 · Dec 6, 2019

dandrummerman21 said:
Is that endmill coated with AlTiN or TiAlN? Or does it just seem like it has that coating because of the light?

If that has one of the coatings I mentioned above, that could be a part of the problem. Aluminum sticks to those coatings, which would have you welding chips to the tool and then the next revolution would snap it off while welding another chip to it.

You would be better off having an aluminum coating (like ZRN), or simply uncoated carbide (that's what I would do for this; cheaper too).

If it isn't coated and it is just the lighting that makes it look like that, Milland has a point.

If it is coated, you can probably still get through with the very expensive tools you already paid for, maybe just lower the rpm some. It would stick less with less heat generated.

FWIW in the future, a couple things you might do instead of this large expensive tool:

1: grind your own radius on a tool.
2: Instead of a large bullnose cutter with 4mm radius, you could buy an 8mm ball endmill for a lot cheaper. Use the ball endmill to finish the corners only. Hell, you could rough your current part further with an 8mm ball and use your bullnose to finish the slot to make it look pretty.
3: buy a HSS tool with radius. Its just aluminum, you can go pretty fast in aluminum with HSS too.

the tool is coated with TiAlN, I was informed this was to be used specifically on aluminium? I guess this is where my lack of experience comes in to play. but yes, I have two more of these tools so i'll continue to use them but slow the RPM down, would you suggest around 4000RPM, or even lower? its clear I need to sort my coolant situation out, the coolant flow isn't great and If I need to keep the cutter cool this needs rectifying. I'm going to order some cheaper tools made from HSS and run some parts with these too to see the difference.

thank you for the feedback, appreciated.

NAST555 · Dec 6, 2019

Are you taking it in one pass?
Remember in the corners it is sort of acting like a ballnose, not quite but imagine it like that, So if I understand your post correctly you are taking 3.5mm depth in one go?
For Aluminium non coated polished carbide is the way to go. Something like this YG-1 E-CATALOG YG are my go to carbide for aluminium.

Also you need to get the coolant really blasting in there as others have said. If you can't then I would suggest that you maybe take it in 4 passes and really crank the speed and feed up.

NAST555 · Dec 6, 2019

Danjones777 said:
If I need to keep the cutter cool this needs rectifying..

In my opinion it is not really to keep it cool but to actually blast the chips away for you don't get them sticking. I have learn the hard way. Your chipped endmill is strange to me, I would have thought that it would be full of melted aluminium and maybe even snap off before that happened.

What brand are those? That is crazy expensive!

dandrummerman21 · Dec 6, 2019

Danjones777 said:
the tool is coated with TiAlN, I was informed this was to be used specifically on aluminium? I guess this is where my lack of experience comes in to play. but yes, I have two more of these tools so i'll continue to use them but slow the RPM down, would you suggest around 4000RPM, or even lower? its clear I need to sort my coolant situation out, the coolant flow isn't great and If I need to keep the cutter cool this needs rectifying. I'm going to order some cheaper tools made from HSS and run some parts with these too to see the difference.

thank you for the feedback, appreciated.

Definitely not for aluminum. That's a good coating for steel.

Harvey Tool - Coating Chart for Ferrous and Non-Ferrous Materials

If coated, a ZRN would be your best (cheapest) bet. But uncoated would be just fine for what you are doing.

I seriously believe that you're getting a pretty well welded on built up edge on that corner (note that the chip is roughly where the notch is in your CAM image above), and with each revolution, the next cut knocks off the chip and welds itself to the tool. I really don't think an uncoated tool would have the same issue.

Slowing it down to maybe 3000rpm or even slower, 2000, should reduce the amount of heat in the cut and result in less chip welding. If it was an uncoated tool, I feel like you may be able to do dozens, maybe even hundreds, without much noticeable wear.

I occasionally cut aluminum with a AlTiN coated endmill. Totally not recommended but they do cut. But it would be sparingly (need 5 parts real quick, tool is already in the machine, I have plenty of flood coolant flow at my disposal).

TeachMePlease · Dec 6, 2019

NAST555 said:
Are you taking it in one pass?
Remember in the corners it is sort of acting like a ballnose, not quite but imagine it like that, So if I understand your post correctly you are taking 3.5mm depth in one go?
For Aluminium non coated polished carbide is the way to go. Something like this YG-1 E-CATALOG YG are my go to carbide for aluminium.

Also you need to get the coolant really blasting in there as others have said. If you can't then I would suggest that you maybe take it in 4 passes and really crank the speed and feed up.

I read it as finishing from 7.5mm to 8.0mm final depth.

NAST555 · Dec 7, 2019

TeachMePlease said:
I read it as finishing from 7.5mm to 8.0mm final depth.

Yeah, But I think he is taking 0.5mm off the floor and the full radius in the corners I think.

Search

Largest Manufacturing Technology Community on the Web

Search

16MM carbide bullnose cutter 4mm corner radius - young CNC programmer issues!

Danjones777

Plastic

dandrummerman21

Stainless

Hardplates

Stainless

GENERALDISARRAY

Hot Rolled

Danjones777

Plastic

TeachMePlease

Diamond

Danjones777

Plastic

Danjones777

Plastic

Milland

Diamond

Danjones777

Plastic

dandrummerman21

Stainless

Danjones777

Plastic

NAST555

Stainless

NAST555

Stainless

dandrummerman21

Stainless

TeachMePlease

Diamond

NAST555

Stainless

Similar threads