What's new
By:

Machines that are Tiny and Building More Machines doing "Bigger" Things...

silver2row

silver2row

Senior Member
Hey There,

I went to the hardware section of the site and felt out of place. I think General Discussion is fine for this one...

So, I went to route some ABS today, i.e. not too long ago. Anyway, the bit melted the ABS after about four minutes of routing.

It is a smaller bit, i.e. about 1/16" or 0.0625". In mm, that is roughly 1.59mm. So, this is an extremely small bit with four flutes. I am thinking of moving about 500mm/sec^2 on XY. The part is just some logo for a business.

Side note here...Has anyone used the .stp export in Alibre to handle electrical parts for Kicad v10.0.0?

Okay and back to business here with the melting of the ABS...

This is a small machine that does not move too quickly and is a terrible machine for efficiency. Anyway, I use it to test particular things on a small scale from programs and software to different controllers and motors along with motor drivers.

Does anyone have any methods, machinists here would easily answer I believe, for NOT melting ABS on about 8500 RPM at 500mm/sec^2? I will double check the gcode but I am pretty sure I am supposed to be moving at 500mm/sec^2.

The Z-Axis is different and slower, i.e. roughly 45mm/sec^2. Any and all contributions are welcomed. I am posting. So, have at it. Oh! The model used is just some lettering around a photo in gcode.
 
Do not laugh too hard but here it goes:

acc.jpg

That is what happened. So, either the RPM of the spindle is too fast or the mm/sec^2 are a bit slow.

I still need the advice. I see people using 5000 RPM. I would need to dial in this machine a bit more to handle the exact RPM given at what dial location on my controls.

The spindle is just a DC motor with PWM drivers handling the speed and/or rotations per minute. Anyway, I could be wrong and I will learn either way.

I read that 5000 RPM is okay but that larger diameter, HSS end mills work just fine but I am seeing something different. Oh and this is a sheet and not a block or large piece. It is a flat sheet at 1/8" thickness. The sheet was meant for laser engraving and/or laser cutting with a gas laser. At least, that was the ole idea.
 
We machine a fair bit of plastic, mostly POM. We use the same cutters (carbide) as for aluminium with similar speeds and feeds (maybe slightly faster) so for example Ø3 endmill at 12000rpm and 1500mm/min. Values have been scaled down to suit our max spindle speed of 12000rpm. Obviously you'll need to start with whatever values the manufacturer recommends. Use PLENTY of coolant!
 
What you're experiencing is chip recutting. ABS is a very difficult material to mill for that exact purpose. Now, another thing is that your rpm and feed combination is creating very thick chips. Thick (compared to the tool) are evacuated with more difficulty and end up welding on the flutes.

So, 5000rpm and 500mm/sec(not^2) is too slow. Either more rpm or less feed. Look up feed per tooth and chip load calcs.
This is a great resource.

CNC Cookbook - The Ultimate CNC Machining Resource

CNC Cookbook is the leading online resource for CNC machining software and expertise. Providing comprehensive tools, resources, and information to help CNC machinists of all skill levels optimize their workflow and improve their machining capabilities.
www.cnccookbook.com
www.harveyperformance.com

Selecting the Right Plastic Cutting End Mill - In The Loupe

Our Selection Guide will help you to select the right Plastic Cutting End Mill for your job - a pivotal first step to avoid wasting shop resources
www.harveyperformance.com www.harveyperformance.com

But the best advice here is... Single tooth carbide for plastics. No coating. For plastics, more teeth (flutes), more problems.

And follow the manufacturer's feed per tooth guidelines for the tool you have and for the material you're cutting. Start by going through the manufacturer's speeds and feeds catalogues. When you get a feel for your machine, starting noting down the combinations that work for you and build your own library. Oh, and if a manufacturer does not provide a set of speeds and feeds for the tool you have and for the material you want to cut, it means it's not recommended for that material. Don't use it then.

Super Important: Chip evacuation. Blow air from a compressor towards the engaged part of the tool. Either by hand or by fixing a tube to the milling head. See coolant setup for CNC routers. They can also be used to connect to shop air.
www.mcmaster.com

McMaster-Carr

McMaster-Carr is the complete source for your plant with over 595,000 products. 98% of products ordered ship from stock and deliver same or next day.
www.mcmaster.com www.mcmaster.com
 
Use this at your own peril! I am not liable for damages or injury!!! I am REALLY NOT!!! Remember that! No training or support provided!!! This is milling only!

Now, these values are slightly conservative for milling on a medium CNC mill, Haas VF2, smaller Doosan Mynx, etc. For a small router these might be too... Optimistic.

For plastics go for the Aluminium material category in the drop down. It's supposed to be Aluminium and non-ferrous materials.

If you go to the 2nd sheet you can change the numbers and then this spreadsheet gives recommendations that work for you.

But if you post a question here, I'll answer when I can
 

Attachments

silver2row said:
So, I went to route some ABS today, i.e. not too long ago. Anyway, the bit melted the ABS after about four minutes of routing.

It is a smaller bit, i.e. about 1/16" or 0.0625". In mm, that is roughly 1.59mm. So, this is an extremely small bit with four flutes. I am thinking of moving about 500mm/sec^2 on XY. The part is just some logo for a business.
...
This is a small machine that does not move too quickly and is a terrible machine for efficiency. Anyway, I use it to test particular things on a small scale from programs and software to different controllers and motors along with motor drivers.

Does anyone have any methods, machinists here would easily answer I believe, for NOT melting ABS on about 8500 RPM at 500mm/sec^2? I will double check the gcode but I am pretty sure I am supposed to be moving at 500mm/sec^2.

The Z-Axis is different and slower, i.e. roughly 45mm/sec^2. Any and all contributions are welcomed. I am posting. So, have at it. Oh! The model used is just some lettering around a photo in gcode.
Click to expand...

(ob. discl., I work for Carbide 3D)

We have a video series on this:


and the usual suggestions are:

- single flute tooling
- a light application of diluted dish soap on the surface to help break chips
- adjust feeds and speeds to arrive at a suitable chip size/formation
- consider an air blast if possible

FWIW, I just use the Carbide Create defaults and it "just works" (so long as I actually match material --- "hard plastic" works on cast acrylic but not extruded acrylic for example).

Used to be I'd look up up specific feeds and speeds using a trial of G-Wizard from CNCcookbook.com, but that program is no longer available (though the excellent information on the site was fortunately preserved).
 
silver2row said:
Hey There,

I went to the hardware section of the site and felt out of place. I think General Discussion is fine for this one...

So, I went to route some ABS today, i.e. not too long ago. Anyway, the bit melted the ABS after about four minutes of routing.

It is a smaller bit, i.e. about 1/16" or 0.0625". In mm, that is roughly 1.59mm. So, this is an extremely small bit with four flutes. I am thinking of moving about 500mm/sec^2 on XY. The part is just some logo for a business.

Side note here...Has anyone used the .stp export in Alibre to handle electrical parts for Kicad v10.0.0?

Okay and back to business here with the melting of the ABS...

This is a small machine that does not move too quickly and is a terrible machine for efficiency. Anyway, I use it to test particular things on a small scale from programs and software to different controllers and motors along with motor drivers.

Does anyone have any methods, machinists here would easily answer I believe, for NOT melting ABS on about 8500 RPM at 500mm/sec^2? I will double check the gcode but I am pretty sure I am supposed to be moving at 500mm/sec^2.

The Z-Axis is different and slower, i.e. roughly 45mm/sec^2. Any and all contributions are welcomed. I am posting. So, have at it. Oh! The model used is just some lettering around a photo in gcode.
Click to expand...
I would reiterate what Will Adams and Ex Machina have said, you are getting rewelding and reattachment of the ABS plastic, this is very common with that type of plastic.

POM type materials which Big Seb talked about machine beautify, even with tools designed for aluminium, the swarf does not reform with these materials.

Swarf evacuation and single flute tools will massively help in minimising the rewelding.

Be careful of too high RPM as well, with your 4 flute 1/16" cutter there was not much space for the swarf in the slot and with the RPM then heat built up. Will Adams also mentioned this. Generally for a small cutter like 1/16" you would run high RPM if the material does not try to reform after the cutter, I have used upto 30,000 rpm with PCB cutters machining carbon fibre, here is a very light weight machine that I had cutting carbon fibre with 1/16" cutters at 30,000 rpm.

I find with small machines such as you are talking about that you often have to develop your own feeds and speeds based upon what you hear and see as the cutter works. A feed and speed that is good for a full on machining centre will not be the same as for a hobby type gantry router.
 
"Single tooth carbide for plastics. No coating. For plastics, more teeth (flutes), more problems," is what you said @Ex Machina . I see people are agreeing and for a certain reason.

Single flute. Done. Now, I need to find them first. I usually mess with wood. So, no real issues on the fluting aspect to the end mills so far. I am sure differences in tolerances and hardness matter for which type of endmill to pick.

And to @bigseb , I might think of coolant. Would something like ID threading oil be okay? I can always use air (sort of). This small machine sometimes is my go to for testing. So, I can actually physically remove it by hand, well two of them, and then replace it in place once more.

I have been reading some and watching some videos. The general consensus states single flute. So, I will go with this fact.

I cannot remove the plastic from the darn endmill. Blah. Off to boil or get some mighty precise cutters to chip at it.
 
Maybe or a soldering iron. It has hardened well. I see what you are referencing from what I said, i.e. the precision cutting tool like snips. I do not want to chunk it. It is one of my nice end mills (I think). I need to double check the insignia on the side(s).

Odd days. It cuts hardwood and softwood easily. Now, since it is 0.0625", it really takes forever to finish projects that are being tested. Oh and I just looked over the photo I provided.

It is a HSS endmill that came cheaply. I bought a bunch of them in a pack for $30.00. So, I may just chunk it. Everything was going nicely. I made some proper cuts and then the weldment happened.

The weldment is stronger than the ABS sheet.

I had to replace a soldering iron recently and this thing came with one chisel tip that is a little under 5/16" in diameter or roughly 7mm. Once it is heated up, that thing can solder just about any solder I carry here locally.

I do not know why this hardened goo got to me so much. Well, I ruined an endmill and a fine piece of ABS sheet. That is probably why now that I think about it.
 
silver2row said:
And to @bigseb , I might think of coolant. Would something like ID threading oil be okay? I can always use air (sort of). This small machine sometimes is my go to for testing. So, I can actually physically remove it by hand, well two of them, and then replace it in place once more.

I have been reading some and watching some videos. The general consensus states single flute. So, I will go with this fact.
Click to expand...
Single flute cutters are great, especially when using smaller diameters. We use the aluminium cutters because a) we have them and b) after trial and error found good conditions for them. Also helps keep our tool numbering system as small as possible.

Some here have suggetsted air... that blows the chips all over the show. Coolant not only stops the cutter and material from overheating but also flushes it straight to the swarf conveyor and into the skip.
 
I have V-bits only outside of single flute endmills. I will think about investing in these endmills soon. I think my worry at first was due to the, and melting of course, set up.

By set up, I mean that my fixtures and holding was mediocre at best. It was not how I should have set things up to start to cut.

...

With that in mind and since I have no single flute endmills on hand right now, I am retrying the whole shebang with better fixtures and holding. Now, are my fixtures and holding at 100% satisfactory? No, I can say it. No, my fixtures and holdings are mediocre. I needed to have two more fixtures to hold this ABS Sheet in place. I went with a line of parts underneath the ABS Sheet. So, instead of a X of a shape of holdings and fixtures, I went with a line. Oops.

So, as some of you machinists out there may already know...

1. When I hit the far reaches of the part, it gives instead of cuts with the endmill at -X350mm and -Y350mm.
2. At -X350mm and at -Y350mm, I should have had better underneath fixtures for the ABS Sheet.

"Learning slowly!"

Oh. And to anyone 3D Printing Nylon with Glass Fill, the higher the Glass Fill the better it seems when creating parts for fixtures and holdings.
 
Ex Machina said:
What you're experiencing is chip recutting. ABS is a very difficult material to mill for that exact purpose. Now, another thing is that your rpm and feed combination is creating very thick chips. Thick (compared to the tool) are evacuated with more difficulty and end up welding on the flutes.

So, 5000rpm and 500mm/sec(not^2) is too slow. Either more rpm or less feed. Look up feed per tooth and chip load calcs.
This is a great resource.

CNC Cookbook - The Ultimate CNC Machining Resource

CNC Cookbook is the leading online resource for CNC machining software and expertise. Providing comprehensive tools, resources, and information to help CNC machinists of all skill levels optimize their workflow and improve their machining capabilities.
www.cnccookbook.com
www.harveyperformance.com

Selecting the Right Plastic Cutting End Mill - In The Loupe

Our Selection Guide will help you to select the right Plastic Cutting End Mill for your job - a pivotal first step to avoid wasting shop resources
www.harveyperformance.com www.harveyperformance.com

But the best advice here is... Single tooth carbide for plastics. No coating. For plastics, more teeth (flutes), more problems.

And follow the manufacturer's feed per tooth guidelines for the tool you have and for the material you're cutting. Start by going through the manufacturer's speeds and feeds catalogues. When you get a feel for your machine, starting noting down the combinations that work for you and build your own library. Oh, and if a manufacturer does not provide a set of speeds and feeds for the tool you have and for the material you want to cut, it means it's not recommended for that material. Don't use it then.

Super Important: Chip evacuation. Blow air from a compressor towards the engaged part of the tool. Either by hand or by fixing a tube to the milling head. See coolant setup for CNC routers. They can also be used to connect to shop air.
www.mcmaster.com

McMaster-Carr

McMaster-Carr is the complete source for your plant with over 595,000 products. 98% of products ordered ship from stock and deliver same or next day.
www.mcmaster.com www.mcmaster.com
Click to expand...
The CNC Cookbook link is a no-longer viable option from what I checked. The fellow that manages the cookbook has passed away.

The harveyperformance.com link seems okay. I will read up more.

I got a funny video of this tiny machine doing things:


I am four hours in now. It seems that the machine is doing its business better than before this time. I will see what has happened when I remove the shavings from the ABS Plate.

Anyway, I appreciate you and your time. The links from your youtube videos have been helpful.
 
It is a bucket with a CNC in it! The reason I am choosing this controller and machine...

1. Easy and quick testing
2. So, I do not mess up better machines
3. And so I do not mess up more expensive controllers while learning...

Outside of jigs and fixtures, this Nylon-GF produced by COEX could be a fun thing to machine too. I will test soon and report back.

So, I can basically solidify the plastics, Nylon-GF, and then machine them to become more than what they would have been with just 3D Printing.
 
Last edited:
You must log in or register to reply here.
Back
Top