Help with Text Necklace

CNC Machines
1

Hi all,
After watching Winston’s video where he makes the carbide 3d text necklace, i’ve been inspired to try making one myself with my pro. I’ll most likely be using a 1/32 endmill but I’m a little worried about breaking it as i’ve never used a 1/32 in metal before. Any tips and tricks anyone could share to make the process go smoothly? I thought i would start with the speeds/feeds from the video and go from there. Thanks!

2
  • small tools don’t like deflection. At all. So keep the stickout to a minimum, and making very shallow passes. A very conservative depth per pass is your best friend when first trying small tools.
  • ideally, check router runout. Micro-machining tools are very sensitive to excessive runout, simply because it will make the actual load on the cutter vary significantly. For example, 0.005" runout may not matter much for a 1/4" endmill, but for a 1/32" endmill it’s 15% of the diameter, so it will end up making the actual chipload vary by +/- 15% over a revolution.
  • In metal, a little lubrication and/or and air jet help. And of course ramping into the material rather than plunging.
1 Like
3

Thanks for helpful reply. I’ve seen talk of ramping instead of plunging in these forums but i’m not quite sure what it means. I suspect ramping is an option in more advanced cad/cam software? I’m pretty new so i’ve been sticking with Carbide Create.

4

Yes, “ramping” means having the tool enter the material along an angled path rather that plunging straight down, and indeed it is an option in other cad/cam software like Fusion360, Carbide Create does not support it (yet). That said, if you go slow for the plunge and use a small depth per pass, it will work just fine.

1 Like
5

Less than 1 hour ago, I finished milling a 1.75 in wide logo in a piece of brass with a shapeoko XL (stock Z) using a 1/32 inch carbide 2 flute endmill. These were raised letters surrounded by a pocket. 24000 RPM, 20 inch/minute feed, 5 inch/ minute plunge. 0.002 inch depth of cut, 0.006 inch stepover. Total depth 0.026 inch. No lubrication, no air; it was throwing dust. No ramping, drawn in Carbide Create. Seems it would do this all day long.(Also, felt like it took half the day). Also did it in aluminum with the same settings first as a test cut, no issues.
Running 10000 RPM,10 inch/minute feed, 0.006 inch depth of cut, broke the bit in test brass within 1 inch of start. It broke in a slot which is impossible to avoid on the first cut. I think the breakage was due to the depth. Your mileage may vary depending on your machine’s rigidity.

1 Like
6

Thanks for sharing your experience, sorry to hear about the broken endmill :slight_smile: Sounds like taking a REALLY shallow depth of cut is going to be one of the key things here. I’m not planning on mass producing these or anything, i’m fine with the job taking some time.

7

This topic was automatically closed after 30 days. New replies are no longer allowed.