Yeah a Haas is like flying a Boeing 747 vs. a Cessna airplane with the M3 (e.g. the stiffness needed to drill on the z-axis), but at around 8:45 of this clip he mentions about self centering point geometry of the drill bit. I have yet to try this and wondered if anyone has tried these bits before.
I'm in pursuit of challenging the existing paradigms of drilling metal with the M3. So far I've had success with using a typical 1/8" drill bit in the dewalt router on the second setting (around 19666 rpm). I was trying to use SFM of 1287, because I found a table 800-1500 for aluminum, but found on this forum a much lower SFM of 262 was good... So I'm not so sure now about this. Anyhow using that, and going down only about 0.5mm could make a large enough hole to use for a drill press. Probably not the best solution, so I'm searching around for something better. I suspect using this bit may have better results, but I'm not sure yet if it is worth the investment to be used with the M3.
Post by Derek the Admin on Oct 15, 2018 5:38:23 GMT
The "ideal" SFM will depend both on the work material and cutter material (IE: HSS vs Cobalt). You just won't be able to hit those low end SFM recommendations. The bottom end of the DWP611 is 16k RPM, so with a 1/8" tool the lowest possible surface speed is 524 SFM. For this reason you are better off with a carbide tool over a HSS tool. Also, as mentioned in the video, the nicer ones will probably be self centering.
Have you tried some very low step peck drilling all the way through the material?
MillRight CNC Staff I do not answer private messages. Please ask questions in public or hit up support@millrightcnc.com
Hi Derek, Oh yes thanks for reminding me that makes more sense... the 800-1500 came from this: www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx And I was at first working with a carbide flat end mill until I broke it, then moved on the a regular drill bit. What I tried was a helix bore to .164" diameter (#8 screw major diameter) using a 1/16" carbide end bit, and it worked for a while. I can't remember what depth I was using, but it was shallow I believe is was 0.02" or less. Perhaps my feed was too fast as well. I think it was 43 ipm.
(I've ordered more bits so I'll give this another shot, but I haven't ran across these self centered bits yet) After breaking the bit, I then used a typical black and decker drill bit set which I believe is hss with black oxide.
I did try a manual jog technique with the hss drill bit where I step down about 0.5mm at a time and listened to the sound to quite down I could successfully drill through the material this way, so if I had only a few holes to do... it would be fine, but there is something that can't be beat about feeling the pressure of a good drill press.
If I had to guess best results for the M3... I'm thinking carbide end 1/8" diameter for 1/8" cullet, 118 degree, self centering geometry... and just go down far enough for the drill press. Would you agree?
Before doing that... I can't remember who said this, but I may just try a carbide 1/8" flat end mill (i.e. the ones I just ordered)... while this may not be the ideal geometry if it works it can save me from doing a tool change, and there is something to be said about that. I want to test something for the team, that is... do a one-pass one-tool 1/8" that etches the contour about 0.01" deep (or less) and then go and make the pilot holes. The idea is quick turn around time on the mill. (less chips to clean up too). The kids may need quick turn-around time to prototype some ideas... they get these with just that one-pass work being done... they can take it to their band saws and drill presses to finish making the parts.
Post by Derek the Admin on Oct 15, 2018 21:58:01 GMT
If you just want to mark for further drill press work then I think you will be fine with just divoting with the 1/8" end mill. I have done that a few times myself when I don't want to do a tool change and needed a hole that size. I'd give that a go. I think that will do what you need.
MillRight CNC Staff I do not answer private messages. Please ask questions in public or hit up support@millrightcnc.com
One thing I'm curious about with a 1/8" divot of an end mill is the how deep I need to make it for a 118 degree drill bit to align, so I've sketched out the geometry of what I'm guessing I should do:
In this sketch, I'm going to use a 118 hss with a 0.164" diameter, and I'm using an arbitrary safe distance before the point of the drill hits. It looks like my depth needs to be at least 0.04" so that the walls of the divot can help guide the drill bit concentric. Does this sound about right?
When testing geometry using 135 degree bit, it only buys 0.01 depth, so it would be at least 0.03"
Post by Derek the Admin on Oct 16, 2018 16:10:49 GMT
I'd use a little trig to verify it. I'd suggest making a right triangle to make it easy to work with. Not 100% requires, but that makes it easier on my brain.
IE: Run a line up the centerline to form one leg of a right triangle that splits the 118 degree angle to 59 degrees. 180 - 59 - 90 = 31, so the other angle is 31 degrees.
We know that half of the 1/8" is 1/16" or .0625". That's the length of one leg of the right triangle we made. We've got a leg length and the angles so we can figure the rest. TAN(31 degrees)= 0.600861.
.0625" * .600861 = .03755" This means you need to be deeper than 0.03755" for the drill to start having side wall to hit.
As I finished calculating that, I realized that you're talking about finishing it with a larger drill bit. I was calculating based on a 1/8" drill following a 1/8" end mill's pecks. In that case, I think just the smallest divot will allow the drill to center itself in the hole.
MillRight CNC Staff I do not answer private messages. Please ask questions in public or hit up support@millrightcnc.com
As I finished calculating that, I realized that you're talking about finishing it with a larger drill bit. I was calculating based on a 1/8" drill following a 1/8" end mill's pecks. In that case, I think just the smallest divot will allow the drill to center itself in the hole.
smallest divot? Like for example 0.0165"?
I picked that depth from a M3 video I caught someone using that depth for contour cut at IPM of 34. I figure if its a safe setting for milling should be safe for drilling.
I guess I was concerned that if the 0.164 drill bit point hit the metal unaligned on a shallow divot it may set that way before the walls of the divot could fix it. I haven't figured out yet why it would work on a shallow case, but if it's been tested to work... I'm all for it, because I don't know how to get HsM express to do what I want it to do otherwise.
As I write this... I think I may know the answer... I'll need to look more closely at the geometry of the flat end mill.
Ok I'm going to experiment with this and see, my gut tells me a tool change is fine, but the real issue for me is some assurance that I don't lose alignment when I do it. So I think I may just etch in the drill points on the first pass with the end mill and then switch tool to this 2956A43 bit from McMaster. I've picked this one because it can also do plastic. Using this on the next pass I can confirm alignment, and the geometry of the divot is favorable to a reliable alignment when using the drill press in post production.
One thing I'd be interested in knowing is the use case of the ball nose bit vs. this bit. I have the ball nose bit, but I'm not sure when I should be using it. I'm guessing for chamfering?
Ok I've got some good starting point test results:
So the 118-degree, self-centering, carbide drill (see previous post for part number)... on a dewalt router using speed setting #4, seems to work great as shown in this video. I'm still working out the software aspect of it though. On this video it completed a 2 pass 0.0165" 0.033" depth, and then I zero the z axis down 1mm more (about 0.04"). I think this may be enough for good divots for the drill press alignment, but after this video I went ahead and went down another 0.5mm and ran same depth 3 times. Now the holes look plenty deep enough.
Based on these tests I think I want to try to target 0.05" depth (1.25mm) using a very slow feed... my theory is that pecking technique is only needed to assist getting chips out, and if it's shallow enough then the pecking approach isn't necessary. The depth of the divot shouldn't have any issue with chips.
I plan to be drilling a lot of holes in the future for FRC, so I want to get a well-defined solution to this, but for the short-term I need to get some other work finished, and then I'll come back to more tests later, and update then.
If anyone else has had good success with m3 and dewalt, drilling 1/8" holes please share... thanks.
