[doublec4]

Hello everyone,

I'm new to the CNC world and I just finished my FLA-100 build. I'm trying to cut some 1/8" thick black abs plastic sheet. I'm using a 1/8" single flute end mill to cut.

My first results were poor, I was trying to cut a simple circle but I ended up with a melted blob and the piece lifted off the table and was vibrating.

Any advice on feeds (down into the piece vs. horizontal) and spindle speed would be great.

Also, when routing profiles in these sheets, should I be using climb or conventional milling?

What depth should I step into the material for each pass?

Thank you for your help!

[neilw20]

Melting? How many RPM? Too many?
Abs blunts a HSS so quick, it will make lots of heat before too long.
If you look at cutter with magnifying glass you will see the rounded off cutting edges.
ABS conducts heat badly so it hangs around. I've found spraying with water helps.
I have found convention milling gives a better finish due to the initial rubbing pressure of cutter burnishes the surface.
Recycling chips, as with other materials, leads to a poor finish too.
Climb milling works OK until the cutter looses it's edge, then it is all downhill.

[doublec4]

RPMs were about 13500, my router can go as low as 8000 if I need to.

I think I may have also stepped down into the material too much. Maybe I would benefit from running a helix pattern at a shallow angle?

[BanduraMaker]

How many flutes on your tool?

[doublec4]

Single flute spiral. This exact tool:

http://www.ebay.ca/itm/380450207661?...#ht_1456wt_906

I got some better results by slowing down the spindle speed to 8000rpm, and xy feed of 750 mm/min. I also only stepped down 0.3mm at a time. There wasn't any melting, but once I got about 3/4 of the way through the material, the bit grabbed and lifted the plastic sheet.

I thought the chips were a bit small so I also tried the same spindle speed, but a faster xy speed of 1000 mm/min but it grabbed the sheet and lifted it right away.

Any help would be appreciated

[BanduraMaker]

Hmmm...That speed of 750mm/min sounds slow but if you've got grabbing...

Is your router pretty rigid? Is your ABS clamped down well? I'm guessing that you're getting grabbing because something is flexing too much but, it's only a guess.

[doublec4]

The router seems pretty rigid. It's an FLA-100 if you're familiar with them (8020 extrusions). I don't really have much machining experience so I don't have much to compare it with.

I'm going to clamp the plastic down better, however, I'm somewhat limited with the profile I have. I will probably just bolt it to my spoil board in whatever areas I can. I don't have a vacuum clamping system.

[Devastator]

Single flute spiral. This exact tool:

http://www.ebay.ca/itm/380450207661?...#ht_1456wt_906

but once I got about 3/4 of the way through the material, the bit grabbed and lifted the plastic sheet.

Any help would be appreciated

I've had better luck on thin flexible sheet by using a downcut bit. The downcut bit keeps the tool from lifting the sheet off of the table. This is what I used to cut ABS recently: Carbide two flute at 8000 RPM, feed~100 IPM, DOC 1/2 tool diameter, climb milling. I got my bits from precisebits.com.

Also, if you have runout in your spindle it can cause melting even with good tooling and feedrates.

[neilw20]

I've made a pressure hold down brush like the big machines use. This stops lift up.
[ame=http://www.youtube.com/watch?v=dAIl0kOLc2Y&feature=player_detailpage&list=UU5HVvtd3BW7aB9xW0qZc1PQ]PCB Drill-router.MOV - YouTube[/ame]

[atwooddon]

Try reducing the router speed and increasing the mm/min settings. If you are getting melting, it typically indicates something is 'rubbing' vs 'cutting'. I had the same problem, and my first guess was to do just the opposite which made the situation worse. Then I read about cutting acrylics and people having problems with the acrylic melting. Solution was to up the mm/min and slow the rpm down. Worked great.

Don

[doublec4]

Thanks for the tips guys.

I ended up with some good results today. I had the spindle speed at the lowest setting (8000rpm) and fastened the four corners of the sheet to my spoil board.

Despite conventional rules, I actually had a cleaner cut with a lower xy feed all other variables remaining the same. When I upped the feed to 1100mm/min, there were thin, ribbon-like pieces of plastic rewelding themselves to the edge. They can be peeled off by hand, or cut off simply with a knife. However, the slower feed rate seemed painfully slow. Maybe I'm still being a bit conservative with the feed? Either way, I machined some clean pieces that were acceptable.

The pressure hold down brush is a great idea and would work really well for this. Since I have the four corners fastened, the hold down brush would keep the center areas from lifting, without having to drill holes for hardware.

I'm also going to invest in some downcut bits. Right now I have a limited selection of tools since I'm just starting. I'll have to diversify my arsenal