I need to make this part (repeatable) and thought to try on the CNC instead of the router table (I’m certain I could make a template and cut with a carbide bit). I.’m just trying to get my head around the process and materials.
The part is about .040 -.060” thick brass. Holes are about .0635” in diameter. I have it modeled in Fusion 360. But what type of brass sheets do I use? What type of bit? And then of course speeds and feeds.
In your picture the right side of the V will be rounded. The left side on the outside will be at the angle you draw it at. The reason is the inside corner cannot get square because of the radius of the bit. You will likely need to file it to get rid of the rounded edge. Others will jump in with F&S and bits to use. Not sure what it is but looks a lot like a 57 Chevy hood ornament. (Well sort of).
Joe,
Take a look at these. Choose one appropriate for you application then we can help with the tooling question.
360 cuts the best but you will need to put a finish on because it tarnishes quickly. Can be cut very easily with carbide and no coolant needed.
I actually need it to tarnish. The one in the pic was plated, but I need polished brass. I will check out the brass you posted.
58 Gibson Flying V Korina?
360 is for you then. It will polish out nice then tarnish perfectly for this application.
McCasser does not have 360 sheets only bars. Should I look else where or go with the 353?
Sorry, you are correct. The 260 should work but let me look into it a bit more tomorrow.
The 353 comes in .063" McMaster-Carr and has a good maintainability rating. Commonly called engraver’s brass. Can be polished and decorative. Not sure about tarnishing. The 260 offers more size’s and could work as well although not as machinable.(probably not that big a deal) They call it cartridge brass so it sounds like it would tarnish like a cartridge. 260 is used quit a bit in musical instrument manufacturing. McMaster-Carr
There will be a color difference between the two and I believe the 260 will be a bit more yellow. The 353 has a bit more copper and look a little more red.
I would lean toward the 260. As far as producing the component you are after, it depends on the equipment in your shop. If you plan to use a CNC router, I would use the painters tape/super glue method on a very flat surface. For the cut, I would use a 4 flute 1/8" to rough and 1/6" to finish. Carbide of course. If you can get these in down cut, that would be best. The reason I say 4 flute is that you want a tight pitch between teeth to reduce the interrupted cut.
Thanks Craig.
Yes I will use my smaller CNC. I will look to order some 260 from McMaster as well as the recommend bits. Any reason to not just use the 1/8” (4) flute bit for rough and final cuts? I suppose I could clean the inside angle with a file and drill the holes on the drill press. Though cutting the holes on the CNC would remove the extra operation.
The only reason I suggested the 1/16" was inside radius and holes. The smaller diameter around the outer perimeter will also leave a nicer finish but if you are buffing, that wont really matter.
found some 260 brass at .0625 which is what the original seems to measure. The string holes are .073 so a .0625 bit should be ok to mill those out. I’ll order the bits and brass soon. If I use the 4 flute carbide 1/16" bit, what would be my speed, feed and DOC be? I have a DeWalt 611 router in my smaller CNC. I think its range is 16k to 25K rpms.
In the Shapeoko table of Speeds/Feeds they recommend a DOC of that calculates out to be 10% of the size of the bit for a 1/4" end mill (.020 DOC) for brass. Would that be the same calculation for the .0625 bit of a DOC of .006?
Do you have a machine that has an ER11 collet spindle in your shop? If so, that’s what I would use. If not, you will want to be sure you do not have run out on a end mill that small. For a .0625", 4 flute solid carbide coated, 500 SFM at .00049" per tooth. So, 30558 RPM and 61.00 IPM. If you are slotting, .021" axial depth of cut. Side milling, .025 radial depth of cut. For the hole, helical ramp with .005 per pass.
Hi Craig,
Yes, my DeWalt 611 has the Precise bits ER collet with lowest run-out they offer. I forget their terminology but its the most precise they have of the 3 collets.
Wow…i wasn’t expecting the feed or RPMs to be so fast. I checked out the calculator. Not sure how you came up with 500 SFM or the .00049 per tooth. The rest makes total sense.
Thanks brother…
Joe
This topic was automatically closed after 30 days. New replies are no longer allowed.
