[user834342]

Hi!
I have a C-Beam based DIY CNC machine and when cutting my last piece the edges or surfaces are very bad. I've have some good results in the past but now not so much. I'm kinda a new to all this so not really sure where to look first in order to solve this.

I've attached 2 photos showing the material and the chips.

Controller: Arduino Due and g2core
Spindle: Makita 700c
Software: Fusion 360

Is my tool blunt?
Backlash?
Bad choice of Fusion 360 operation?
Too high feed rate?

Any input much appreciated!
Thanks

[robwiacek]

Hi!
I have a C-Beam based DIY CNC machine and when cutting my last piece the edges or surfaces are very bad. I've have some good results in the past but now not so much. I'm kinda a new to all this so not really sure where to look first in order to solve this.

I've attached 2 photos showing the material and the chips.

Controller: Arduino Due and g2core
Spindle: Makita 700c
Software: Fusion 360

Is my tool blunt?
Backlash?
Bad choice of Fusion 360 operation?
Too high feed rate?

Any input much appreciated!
Thanks

I’m thinking:
Dull tool ( get new tool)
Too aggressive of a plunge cut ( take smaller steps down)
Dry Cut (maybe add lubricant to smooth cut)


Sent from my iPhone using Tapatalk

[user834342]

OK so it's not something obvious then!?

[user834342]

I had the same problem with a brand new tool so thought it wasn't really the tool.

Here's an example:


I also tried a really slow feed/plunge rate.

[robwiacek]

I had the same problem with a brand new tool so thought it wasn't really the tool.

Here's an example:


I also tried a really slow feed/plunge rate.

Maybe use a Down Cut bit


Sent from my iPhone using Tapatalk

[robwiacek]

Maybe use a Down Cut bit


Sent from my iPhone using Tapatalk

I. Any see how many down passes you use.
If you are cutting 3/16 material..... do 5 light passes.


Sent from my iPhone using Tapatalk

[mactec54]

OK so it's not something obvious then!?

I don't know about that it looks like the build has lots of problems, what are you using for a spindle

Post a photo of the whole machine it looks like you have a rigidity problem plus not using some type of coolant, not all machine builds like this can cut aluminum

[robwiacek]

Post a photo of the whole machine it looks like you have a rigidity problem plus not using some type of coolant, not all machine builds like this can cut aluminum

I agree... there’s a lot of chatter.
But slow down the feed and plunge rates and add a coolant or at least WD-40


Sent from my iPhone using Tapatalk

[robwiacek]

Maybe use a Down Cut bit


Sent from my iPhone using Tapatalk

Yeah but it looks like you should choose a down spiral bit


Sent from my iPhone using Tapatalk

[mactec54]

Yeah but it looks like you should choose a down spiral bit


Sent from my iPhone using Tapatalk

It would not matter what kind of cutter he used if everything is vibrating and jumping around

[robwiacek]

It would not matter what kind of cutter he used if everything is vibrating and jumping around

That has a lot to do with it.
But the consistency in the burr around the top of the cut shows it’s making an even pass with material being pulled out.


Sent from my iPhone using Tapatalk

[mactec54]

That has a lot to do with it.
But the consistency in the burr around the top of the cut shows it’s making an even pass with material being pulled out.


Sent from my iPhone using Tapatalk

What kind of cutter would you use on a machining center to cut aluminum, the same as what he is using, it's all about the machine and coolant, it looks like his cutter is HSS which destroyed it's self in the first 10 seconds of cutting

The Endmill is out of the collet to far, by what is showing in the photo, if he is using a trim router or similar the bearings and router are not designed to cut aluminum, so you can't expect it to be great, but should be better than this if setup right and the machine is rigid enough

[robwiacek]

What kind of cutter would you use on a machining center to cut aluminum, the same as what he is using, it's all about the machine and coolant, it looks like his cutter is HSS which destroyed it's self in the first 10 seconds of cutting

The Endmill is out of the collet to far, by what is showing in the photo, if he is using a trim router or similar the bearings and router are not designed to cut aluminum, so you can't expect it to be great, but should be better than this if setup right and the machine is rigid enough

Agreed. Lubricant is a must.
With the extension of the bit, it is possible to make a clean cut, but it has to be a slower feed rate and a lighter touch.
HSS is not ideal here, eh?


Sent from my iPhone using Tapatalk

[mactec54]

With the extension of the bit, it is possible to make a clean cut, but it has to be a slower feed rate and a lighter touch.

Anything is possible if it is rigid enough, no feed rate or different cutters are going to change the one thing rigidity needed though, the shorter the endmill ( note Endmill not Bit ) is to the collet in this case the better chance the cut will be a little better, but don't expect any miracles, if the machine is not up to it

[cyclestart]

Agreed. Lubricant is a must.
With the extension of the bit, it is possible to make a clean cut, but it has to be a slower feed rate and a lighter touch.
HSS is not ideal here, eh?

Tool extension and lack of rigidity aren't carbide friendly although carbides have become less brittle. Add into the mix a less than ideal spindle.
On my X2 mini-mill I avoid carbides and get much better results than pictured here. Also my max rpm is half a router's min rpm.
Since your router can't be dropped to mini-mill rpm I suggest lots of passes of small engagement and decent feed rate. Lube helps and compressed air if you've got it

Edit/ I looked at a feed/speed calculator for HSS and you're kind of between a rock and a hard place with the available rpm.

[wizard]

That has a lot to do with it.
But the consistency in the burr around the top of the cut shows it’s making an even pass with material being pulled out.


Sent from my iPhone using Tapatalk

You simply do not use down cut bits in Aluminum. Trying to use such would lead to swarf jamming, mill breakage or other problems.

[wizard]

I had the same problem with a brand new tool so thought it wasn't really the tool.

Here's an example:


I also tried a really slow feed/plunge rate.

Well it could be the end mill if you are buying the wrong type of end mill.

Your picture is pretty terrible but the little bit of magnification allowed seems to indicate a lot of chip welding on the cutter. You will need to inspect a little closer to verify but if so you likely will need to lower RPM, address lubrication and feed rates. IF there is significant chip welding you might as well throw the cutter out. In any event the cut surface seems to indicate a lack of cutting and instead tearing which is another chip welding clue.

Frankly I can't imagine a C-Beam based machine being rigid enough to cut aluminum with any quality but ignoring that, you can look at any rigidity related issues the machine may have and address them. In general though Aluminum requires the right feed rates, a cutter with good swarf removal functionality, lubrication (try WD40). I suspect that you are not achieving the right feed rates for the spindle you are using.

Oh there is one other gotcha here, Aluminium varies vastly in the way it cuts baseed on the alloy, temper and other factors. if the bar you are milling today is different than the bar from a month ago you iwll see differences.

[robwiacek]

You simply do not use down cut bits in Aluminum. Trying to use such would lead to swarf jamming, mill breakage or other problems.

I did not know this.
I work primarily in Corian, Wood, Brass
Works in these materials as long as I use air and in some cases lubricant


Sent from my iPhone using Tapatalk

[robwiacek]

I did not know this.
I work primarily in Corian, Wood, Brass
Works in these materials as long as I use air and in some cases lubricant


Sent from my iPhone using Tapatalk

I just looked at a Spiral O bit.
Works beautifully in aluminum.
Check out You Tube



Sent from my iPhone using Tapatalk

[cyclestart]

I also tried a really slow feed/plunge rate.

Imo that's doing yourself no favours. With high rpm of a router that tool has to be kept moving to concentrate the heat in the chips.
When dropping the Z ramping into the cut helps to both maintain speed and clear chips.
Also that rectangular cut is a tough job unless there's a really good way to evacuate chips. Re-cutting chips is the quickest way to get into trouble.


My router has 16mm unsupported round rail on the Z axis, so it's not a very rigid machine compared to a lot of the machines on this site.
For roughing the pocket in this picture: 2 degree ramp down at 20"/min, 0.05 stepdowns with 0.010" radial cut, all radial cuts @ 76"/min.
On the finish cut I went a little nuts and tried 0.015" radial cut at full 0.400" depth @ 76"/min, that didn't go too well Rerunning that tool path 2X cleaned things up a bit.

This was the first time trying metal on my router and if there's a next time I'll try more stepdown and less radial engagement.
The one thing I would be reluctant to try is much slower feed as this was a 1/4" upcut carbide turning near 1000 sfm, about as slow as my router can spin. When the cutting was done the tool and work remained cool or at least not warm.
Attachment 408800.
btw, I was cutting 6061, some alloys are much 'gummier' causing much misery.
Also there's a sticky regarding cutters at the top of this forum and the first 2 pages are a good read.

Some posters frequently cut aluminium on routers so maybe one of them will chip in. I'll stick to a milling machine.