help please cutting small letters from cast acrylic?

[chunkyhammer]

Are you machining the numbers as pockets into the perpex leaving a 0.5mm rad in the bottom corner?

[mark walker]

Hi there, a lot can depend on the cut direction you choose when setting up your tool path. I find that a counter clockwise direction around the letter will suit some materials and clockwise around the letter will suit other materials. I can set this in engravelab don’t know but would think it to be the same with yours. Hope this helps.

Mark 😀

[kong]

You could try lowering your spindle speed, and/or raising your feed speed. Acrylic likes to be worked quickly.

[Westcoast Sign Guy]

Try and post a pic if you get a chance of your finished product. Sometimes it can be the bit (size, geometry), your Z axis setup. From my experience and it’s very short. It can all be on the acrylic too, I found that different makes will bring me different results. I know that 1/2″ diameter bits will bring the best results (damn it, I’m cursed without the Metric system) for edge quality. Vibration is also a big key, any slight vibration and acrylic will bring that out the most. Here’s a pic of the best edging I can get, & I think it’s terrible. But I’m told it looks good for a CNC router.

It has a slight sprocket look to it but not to harsh. Another thing that can make a factor is in the software. Sometimes to many nodes. On the straight cuts you should have the best cuts, if you have problems there it could be your bit type & feed speeds.

Sorry the pics are so huge

[Rodney Gold]

Hiya
Firstly , getting those laser cut is a snap , so thats the avenue I would go for those letters.(tho you cant bevel with a laser)
The ball nose cutter is not the right tool for the job , you should be doing this in 2 passes (maybe more depending on the package and the power of your machine and bit diameter)

Single flute cutters work best on acrylic and you need high rotational spped and high feed rates. Using soapy water as a lubricant and coolant is also ideal.
The ideal strategy would be to use a single flute parallel cutter with a lot of back clearance to plunge and cut 90% deep in a single pass (or do a multiple passes – the general rule of thumb is you can go in only as deep in a single pass as the diameter of the cutting section). Thereafter do a “clean up and break thru” pass , ie go down the remaining 10% and slightly inwards so the cutter cleans the edges and breaks thru.
The ball nose can never give a decent bevel or a “bullnose” type roundness unless you give it very small stepovers. Better for a bevel is to use a bigger diameter 45 degree cutter and follow the cut line tho not to max depth , this will bevel the top edge of the letter.
(you could do this first , however then you are asking the v cutter to remove a LOT of material – which will not be ideal.

Visible toolmarks are symptomatic of many things
1) Bit chatter – IE flex in the tool itself
2) poor interpolation , IE a stepper based machine cannot interpolate arcs in non discrete steps and will not give smooth results
3) Play in the machine itself
4) Too little power , too slow a feed , too slow a speed
5) overheating of the materials
6) blunt tools
7) Too little back clearance – acrylic needs tools that have a lot of clearance for chip ejection.

The best way of buffing the letters is flame polishing them , this will reduce but not totally remove machining marks. Using a coolant/lubricant like the soapy water will reduce your problems dramatically all by itself. If you flame polish and then glue the letters , you are in for problems as it stresses the acrylic and solvents than cause stress cracks or crazing to occur.