Engraving with 1/32 bit.

[Austin Shafer]

So I have to make a bunch of these 3" x 5" signs on 1/4" king colorcore and I'm using a 1/32" two flute bit. what kind of feeds and speeds and what tips do you all have for me to not break a bunch of bits? 26642

[Brady Watson]

Crank your spindle all the way up. Small tools like high RPM.

Adjust VR settings. Change slow corner speed to 40 to reduce jerkiness of direction changes in grabby HDPE. If you get melting in the corners, increase it. If your set speed is less than .4 on any axis (EG - MS,0.3,0.3) then you will need to reduce the first 2 settings in the VR list to the same or lower than your MS values - or the tool will NEVER go that slowly. It will default to these 2 values as the slowest speed.

I would start @MS 0.5, 0.5 with 0.02 pass depth to start. Then add more depth or speed as you see fit. Put your safety glasses on and LOOK at what is going on at the tool tip. Listen. Observe & adjust accordingly. 1/32 tools are not as delicate as you'd think if you get into the right range & don't ask them to cut too deep in one pass.

If you find your motors are making a lot of noise/mid-band resonance @ your target speed, increase or decrease the speed so that vibration doesn't telegraph into the cut. If you raise the MS to get out of the noise, decrease the pass depth.

Just play around...you'll get it. Now get out there and break some bits! ;)

-B

[Austin Shafer]

Wow, thanks for the info Brady. I will give it a shot later today... This is going to take a long time. I have to cut around 40 of these signs and the estimated time for 16 signs is about 14 hours :eek: Hopefully I can slow down enough to get them these signs :p

[Brady Watson]

My advise would be, break it down into smaller chunks. Machining a smaller cluster of parts will give you an opportunity to take a break, but more importantly, it will result in a more consistent engraving because there will be less variation in Z.

Since your machine bed will vary some from one end of the table to the other, there are bound to be some inconsistencies to deal with. This isn't a big deal for 2D cutting, but for something where Z depth is critical (like surface engraving), this variation can ruin your day...If it is off .02-04", the result would be deeper or shallower cuts in the parts.

Think small batches...it doesn't really take any longer & quality control is way better.

-B

[curtiss]

from the font you are using, you might have some trouble with the "e" chipping out...

In Corian with a 1/32nd bit, I usually go with two passes .02 deep each... if I go much deeper the e's usually chip out.

Sometimes you have to run the tool path twice to clean it out. I would have a few spare bits...

[Austin Shafer]

Well, got 7 of them cut and it took over an hour a piece :eek: no broken bits though ;) thanks guys!

[Kyle Stapleton]

Must be some spendy signs.

[Austin Shafer]

Not sure actually I just make the stuff lol We make commercial playground equipment and now this is just another thing we can make in house.

[joe]

Geeees, this sounds like a financial up hill climb.

Joe

[scottp55]

Austin.
Never cut the stuff or used the bit, but remember someone(TJ?) saying they liked the bit.
Maybe try to see if times come down if making many of those?
https://www.centuriontools.com/router-bits-toolcase/solid-carbide-wood-router-bits.html?pcn=V-Carve%20Bits&pid=740
scott

[Austin Shafer]

So far so good! It keeps me busy all the time. If I am completely caught up on parts then my down time I can cut a few signs at a time. Thanks Scott, it looks like those bits are a little big for these letters though.