The endmill used is entirely different. Reddit post guy used single flute 1/4 inch.
Still impressive.
3 Likes
Have you considered V-bits ? for engraving text/symbols on a 10x10mm surface, they would probably work better than a 1mm endmill (unless you specifically want to go for a “round” font). Also since you mention “inlays”, v-carving would be easier ? (it being tolerant to small dimensional errors)
If you go with square endmills, I would favor low flute count for chip evac (and I’m really curious to see what a 1mm 4-flute looks like?..), aim for 0.001" chipload as usual, start by shallow test passes, and then increase DOC until the machine tells you it doesn’t like it anymore.
3 Likes
Hallo Jon,
I have a Nomad and cut symbols and engravings into brass regularly.
My current go-to for engraving is this v-shaped ball end mill:
I cut either 0.1mm or 0.2mm with a 0.05mm depth-of-cut, usually slowly at around 200mm/min, and get really nice results with quite a bit of detail. This fellow lasts a reasonable amount of time, too.
For cutting the brass itself (this depends on which brass you have) a single flute 3.175mm can cut 0.2mm-0.25mm per pass pretty well at around 200-250mm/min.
The type of brass matters… CZ121 is nice and soft and cuts well with these. Harder brass will mean you have to pull back a little on the feed rates, in my experience.
5 Likes
Thanks for all the replies, since looking at this and doing some further follow up ready based on feedback, i spoke to the shop foreman (my wife) who Green Lit the P.O to buy lots of different end mills for experimentation,
Plus the other cheap fle bay ones. i have the best wife ever, i said in passing today i would really like to get a bigger 8x4 CNC, just coffee talk, and got a “my love it it make you happy get what you want!, but start with these bits and see how you get on”
Thanks for all the help i will put some tests up here!
Jon
3 Likes
Thanks for the shout out Jon!
Here are the 2 mm flat end mill and 1 mm ball end mill I used for brass part for the box (Supplier is based in the UK):
Hope you share some photos when you have finished brass parts coming off the machine!
4 Likes
lol i got these from them too, honestly going to have my end mils than brass to cut lol thanks for the link!!
2 Likes
I am curious why you would use a down cut bit on brass won’t that pack the chips into the cut?
2 Likes
@Able I am sorry i would have thought that was very obvious?? as in obviously i have no idea what i am doing :)- so here is my thinking, as i am going to rough cut this first pass, and having watched / read somewhere that down cut on metals can leave a really good finish on the surface i thought i would get one of them too, if my thinking is flawed please do not hesitate to pass me back the noob hat, i wear them with pride 
1 Like
As long as the chips have a place to go it should do fine just avoid any deep pockets or cuts where the chips can pack up. If you use an up cut to rough then finish with a down cut there should be room but you can always use a quick air blast to periodically clear the chips. Duster computer cleaner spray is an option if you don’t have a compressor.
2 Likes
So like a kid at Christmas these turned up. And I want to use them all at once lol, time for a serious test plan!
3 Likes
I will say a prayer for the 1mm end mills may they have a long and productive cutting life.
I am excited to see the finished project.
1 Like
Just a reminder for metals - be sure to make sure you have suitable clamping or adhesion!
I’m averse to double-sided tape because it’s a mess and when the stock heats up it melts and slips… and the super-glue-and-masking-tape thing has not worked well for me (my fault no doubt).
So I usually use tabs in the model. But I try to make them as thin as possible, and often too thin. Yesterdays prototype effort saw the top piece fly off during the final 3.175mm cut of 1/8" stock and wreck the top protrusion on this gizmo.
6 Likes
Asking a Baguette for confirmation about imperial to metric unit conversion is just asking for trouble 
But yes, 0.0254mm. For some weird reason I’m more familiar with ipm units for feedrate now, so I stick to imperial chipload values. Since I’m also a sucker for single flute endmills when cutting metal, it makes for very simple napkin computation of the feedrate (0.001" x 1 x RPM = Feedrate, so e.g. 24kRPM => 24ipm). But then of course there’s chip thinning and miscellaneous other factors.
2 Likes
that piece is beautiful. What are the overall dimensions on that?
Not sure if your question is for Jon or the image I posted… but if it was for the image I posted, it’s 56mm * 45mm * 7mm.
Gerry,
thank you for getting back to me, I appreciate it. I’m super new to the forum (haven’t actually purchased the Shapeoko yet, but I am shortly), and wasn’t sure if you would see the question. I was very interested in the piece that you had created as it had the look of items I plan to make. My plan is to cut championship belt plates from brass on the machine. They will have recessed area for paint (about .040" deep) and some other detail work. I have made similar items before, but using acid engraving. It’s just too messy and unpredictable. Then the step where to get the contour shape, I’d have to get a metal cutting bandsaw. I’m trying to simplify things.
Again, thanks for getting back to me.
Gord
1 Like
Welcome Gord, and best of luck with your aspirations!
That item is actually pretty small compared to a champion belt plate - less than 2" tall and the engravings are 0.2mm (0.008") deep on 1/8" brass. Note that it was made using a Nomad… Hopefully with the larger size of your belt plates, the Shapeoko can manage to cut sufficient detail for the look you are after.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.