Milling Alumium sheets --> sticky chips

reyntjensm · Mar 8, 2021

Hello everyone,

I'm trying to mill aluminium sheets(2mm thick) and i'm having issues with sticky chips.
I have to insert some tabs in my milling program. After some tabs the chips build up resulting in a bad finish. I would prefer not to use any liquid cooling since i have a mdf waste board below the aluminium sheets. I use compressed air to blow the chips away. The tool is a single flute PCD tool(5mm) with 900mm/min feed spinning at 18000rpm and 300mm/min plunge rate
I have attached my aluminium specs and a picture of the bad parts. Can anybody help me solve this issue?

Larry Dickman · Mar 8, 2021

I have no idea what alloy you're working with, but I'm assuming it's soft and gummy, like 3003. I had to make a bunch of panels with it years back. I had the best luck roughing them out using a template and a power nibbler.

reyntjensm · Mar 8, 2021

The alloy is called AW-1050. It's 99.5% alu and it's "half hard". I have to mill 80 sheets of 1500*5000mm so it's not an option for me to do this manually.

DanielG · Mar 8, 2021

A few thoughts:

1) Some companies, like Onsrud, make router bit especially for cutting soft aluminum alloys. Since your alloy is 99.5%, might be worth trying. 63-400

2) Are you using an upcut or a downcut router bit? If upcut, are you pulling up the sheet ever so slightly when you plunge?

3) What happens if, after the tab, you ramp back down, rather than plunging. This test would at least isolate where the problem occurs.

Mtndew · Mar 8, 2021

reyntjensm said:
Hello everyone,

I'm trying to mill aluminium sheets(2mm thick) and i'm having issues with sticky chips.
I have to insert some tabs in my milling program. After some tabs the chips build up resulting in a bad finish. I would prefer not to use any liquid cooling since i have a mdf waste board below the aluminium sheets. I use compressed air to blow the chips away. The tool is a single flute PCD tool(5mm) with 900mm/min feed spinning at 18000rpm and 300mm/min plunge rate
I have attached my aluminium specs and a picture of the bad parts. Can anybody help me solve this issue?

View attachment 315859
View attachment 315860

Spray it with WD-40 along the toolpath, it shouldn't hurt your waste board underneath I wouldn't think.
Or get a cold air gun and have it about an inch away from your cutter at all times.

reyntjensm · Mar 8, 2021

DanielG said:
A few thoughts:

1) Some companies, like Onsrud, make router bit especially for cutting soft aluminum alloys. Since your alloy is 99.5%, might be worth trying. 63-400

2) Are you using an upcut or a downcut router bit? If upcut, are you pulling up the sheet ever so slightly when you plunge?

3) What happens if, after the tab, you ramp back down, rather than plunging. This test would at least isolate where the problem occurs.

I will have a look at Onsrud. Thank you.

What do you mean with up or downcut? I plunge into the sheet but it doesn't move.

I could use ramped tabs but they should be very long otherwise the results are equal

reyntjensm · Mar 8, 2021

Mtndew said:
Spray it with WD-40 along the toolpath, it shouldn't hurt your waste board underneath I wouldn't think.
Or get a cold air gun and have it about an inch away from your cutter at all times.

The waste board is mdf. It sucks up the lubricate and deforms. So i don't want to use it. Should a cold air gun make such a big difference? I think it has something to do with the settings/tool i'm using.

Mtndew · Mar 8, 2021

reyntjensm said:
The waste board is mdf. It sucks up the lubricate and deforms. So i don't want to use it. Should a cold air gun make such a big difference? I think it has something to do with the settings/tool i'm using.

Did I say pour the WD-40 on with a 5 gallon bucket?

DanielG · Mar 8, 2021

reyntjensm said:
What do you mean with up or downcut? I plunge into the sheet but it doesn't move.

Upcut vs downcut is what direction the spiral of the flute is. "Normal" cutters are upcut; they want to pull the part off the table. A downcut cutter has a reverse spiral so it pushes the part into the table. They are great when using vacuum/tape workholding and your grip on the sheet is marginal.

reyntjensm said:
I could use ramped tabs but they should be very long otherwise the results are equal

Assuming your tabs are 1mm high, a 2 degree ramp angle would take 29mm to get back to full depth. Does going to a shallow ramp angle solve your chip problem? If it does but you want a smaller tab, you can always ramp back down to depth and then reverse to make the tab smaller.

Mike1974 · Mar 8, 2021

I would think any air gun close to the cutter would be an improvement. You said you are blowing the chips away, constant, or intermediately?

here is a cold air gun if not familiar -

https://www.mscdirect.com/product/details/09406026

Hardplates · Mar 8, 2021

Mtndew said:
Did I say pour the WD-40 on with a 5 gallon bucket?

LOL ^^

I've never really tried to push aluminum without coolant or a little light oil. But maybe DLC coatings work well without coolant? I know they will run stupid high SFM

Perry Harrington · Mar 8, 2021

Are the chips merely staying in the path or are they sticking to the piece you are cutting out?

I'm assuming this is a CW toolpath and you are climb cutting?

Is the machine executing a decel move right before the tab, or is the motion constant?

I was thinking EN-1050 was a metric grading until I looked it up, it's a pure form of Al, similar to 1100 welding rod.

If the chips are welding to the piece, I'm betting it's because the toolpath is slowing down before the tab and it's causing the bit to rub because the chipload is not high enough.

Perhaps it's as simple as unchecking a box in your CAM processor to not perform decel moves before tabs? Maybe running a higher chipload will be a simple fix?

I know that a lot of these Al setups use Isopropol Alcohol as a lubricant and coolant, plus it evaporates very quickly. Perhaps that is an option for you with air blow? Since it will evaporate so quickly it may not raise the grain on the MDF spoil board.

If you intend to do a lot of jobs like this in the future, perhaps investing in an HDPE or UHMW spoil board would be wise, since they won't be affected by coolant.

Then again, maybe Onsrud has some magic tool that will fix all of this, I prefer to solve the process problem than spend money on an exotic tool.

G00 Proto · Mar 8, 2021

We used to machine mountains of 5052 Aluminum sheets. I never could get it not to load up and eventually friction stir weld without oil. A bit of WD-40 worked for short runs, douching it with cutting oil worked the best. If I absolutely had to machine it dry, I would be experimenting with single flute, deep gullet tools and at minimum air blast or old school Kool Mist. I still think it'll load up, but you might have a fighting chance.

reyntjensm · Mar 8, 2021

DanielG said:
Upcut vs downcut is what direction the spiral of the flute is. "Normal" cutters are upcut; they want to pull the part off the table. A downcut cutter has a reverse spiral so it pushes the part into the table. They are great when using vacuum/tape workholding and your grip on the sheet is marginal.

Assuming your tabs are 1mm high, a 2 degree ramp angle would take 29mm to get back to full depth. Does going to a shallow ramp angle solve your chip problem? If it does but you want a smaller tab, you can always ramp back down to depth and then reverse to make the tab smaller.

it's a single flute PCD tool. It doesn't have any spiral. The software to control the cnc is not that sophisticated. But it's a good point, i will try to do something like that

reyntjensm · Mar 8, 2021

Perry Harrington said:
Are the chips merely staying in the path or are they sticking to the piece you are cutting out?

I'm assuming this is a CW toolpath and you are climb cutting?

Is the machine executing a decel move right before the tab, or is the motion constant?

I was thinking EN-1050 was a metric grading until I looked it up, it's a pure form of Al, similar to 1100 welding rod.

If the chips are welding to the piece, I'm betting it's because the toolpath is slowing down before the tab and it's causing the bit to rub because the chipload is not high enough.

Perhaps it's as simple as unchecking a box in your CAM processor to not perform decel moves before tabs? Maybe running a higher chipload will be a simple fix?

I know that a lot of these Al setups use Isopropol Alcohol as a lubricant and coolant, plus it evaporates very quickly. Perhaps that is an option for you with air blow? Since it will evaporate so quickly it may not raise the grain on the MDF spoil board.

If you intend to do a lot of jobs like this in the future, perhaps investing in an HDPE or UHMW spoil board would be wise, since they won't be affected by coolant.

Then again, maybe Onsrud has some magic tool that will fix all of this, I prefer to solve the process problem than spend money on an exotic tool.

The tool doesn't slow down. problems arise when the tools plunges into the metal after the tab.
Isopropanol is indeed an option...
I also want to avoid coolant since this will need an extra cleaning step for the next production process i'm using these sheets for.

reyntjensm · Mar 8, 2021

Mtndew said:
Did I say pour the WD-40 on with a 5 gallon bucket?

No, but this will shorten the life of the mdf plates. I need to mill this almost 24/7. It would also need extra cleaning. The PCD tool i'm using doesn't need any lubrication according to manufacturer

Perry Harrington · Mar 8, 2021

reyntjensm said:
The tool doesn't slow down. problems arise when the tools plunges into the metal after the tab.
Isopropanol is indeed an option...
I also want to avoid coolant since this will need an extra cleaning step for the next production process i'm using these sheets for.

The Isopropanol will not leave a residue, it will evaporate.

I think your biggest problem is your cutter. You should be using a spiral up cutter for this, not a straight flute.

You can probably call up Datron and purchase cutters directly from them, they have a proprietary design that sounds ideal. And since you are cutting 1050 the abrasive wear will be negligible.

Look here: Single Flute End Mill - DATRON

DanielG · Mar 8, 2021

reyntjensm said:
it's a single flute PCD tool. It doesn't have any spiral. The software to control the cnc is not that sophisticated. But it's a good point, i will try to do something like that

If your workholding will stand it, an upcut tool should really help with chip evacuation. You can still use a single flute tool; they call them O flute tools. That's the letter "O", not the number zero; I didn't get that at first and was very confused about the naming.

M. Moore · Mar 8, 2021

It looks like your cutter is performing well except right after the tab if I understand correctly.
Could you try and move over 1 or 1.5mm after a tab and cut for 75mm, then come back and recut on spec?
This may give some room for chip clearance? Just a short version of rough and finish cut.
The photo shows the same effect as when routing wood, the chips back up in the cut as they have nowhere to go.

Second option would be to have them laser cut, but there is no fun in that.....

Milling Alumium sheets --> sticky chips

Plastic

Titanium

Plastic

Stainless

Diamond

Plastic

Plastic

Diamond

Stainless

Diamond

Stainless

Titanium

Hot Rolled

Plastic

Plastic

Plastic

Titanium

Stainless

Titanium

Similar threads