Bits to purchase next

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

Bits to purchase next

Postby tshelb619 » Tue Nov 28, 2017 11:11 am

Hello,

I am looking to purchase a few more bits to add to what I have started out with. I have been learning my Shark HD4 and have been using the 90deg that came with it as well as a 1/4 end mill.
Looking for recommendations for a few more different types of bits for various applications including cutting out smaller letters as well as detail work and hogging out material.

Any suggestions?

Thanks!
tshelb619
 
Posts: 3
Joined: Fri Sep 01, 2017 11:50 am

Re: Bits to purchase next

Postby Kayvon » Tue Nov 28, 2017 11:41 am

1/4" and 90deg V are a good basic starting set. I find myself using a larger cleaner bit (3/4") for both leveling and taking away large amounts of material. I also use a 60 degree V bit so much that it's my preferred V bit for its deeper cuts.

If you plan on doing any 3D work, you'll want a small rounded end bit or a tapered bit. Ultimately, it all depends on what you intend to make.
User avatar
Kayvon
 
Posts: 271
Joined: Tue Oct 21, 2014 11:46 pm

Re: Bits to purchase next

Postby tshelb619 » Tue Nov 28, 2017 11:59 am

The 60deg v bit was actually one I was looking hard at getting next so thank you so much for that input. As far as what I intend to make, I have been trying to cut out letters and find that either my tabs are not big enough or the end mill I am using is too big for the font and size maybe? It either kicks pieces out and messes up the letters or ends up running together. Any suggestions on a better font or style for say family name signs? I want to be able to both engrave and cut out letters in various fonts.

Thanks again!
tshelb619
 
Posts: 3
Joined: Fri Sep 01, 2017 11:50 am

Re: Bits to purchase next

Postby Kayvon » Tue Nov 28, 2017 6:06 pm

How large are your signs? Post a picture of the VCarve preview and a picture of the actual result and I think we can give you more exact answers.

As a rule of thumb, your final product won't look better than the preview. If you see the bit isn't able to reach tiny corners in the preview, it's a bit-size vs font-size problem. If the preview looks fine, but you're losing pieces of your product, it's probably a tearout problem and it's probably related to feed rates. Again, pictures will help give a more exact answer.
User avatar
Kayvon
 
Posts: 271
Joined: Tue Oct 21, 2014 11:46 pm

Re: Bits to purchase next

Postby Rando » Mon Dec 04, 2017 6:06 pm

My progression through bits included the following, some of which you might find useful. I've excluded the router-bit, carbide weld-on style, since I never like those even on a router ;-).

1) End-mills in general. Moving to solid-carbide, pro-level end mills changed everything for me, making metalwork possible. I started with the flat-bottomed, pointy-tip variety.

2) Extended-length 4-flute finishing bits: these give a mighty smooth finish, but are of questionable use in a Shark, because the long flutes tend to cause pretty big deflections. These are the ones where the flutes are really long.

3) Specific-diameter carbide drills. Getting a (wide) variety of these small drill bits, from 0.019" to about 0.200", means that I can easily do Printed Circuit Board drilling. The smaller diameters are susceptible to breaking due to too-fast plunge rates, but I've successfully drilled hundreds of 0.019" holes with a single drill bit...albeit delicately ;-). These are often cheaper by the 10-pack, which is how I usually get mine.

4) Small-diameter end-mills. I do a lot of "part" machining, and I ended up needing endmills in 1/8", 1/16" and 1/32" diameters for some really detailed features in a product. They're rarely used, but when you need them, you need them. Just remember: they don't take stress very well....but, they DO also come in 10-packs :D.

5) Radiused endmills. OMG this improved my life! By grinding a small (0.010-0.030") radius on the flute tips, it makes things much better. Stronger tips for breakage is rare. Deflection diving into the material is almost eliminated, and it gives a nice small fillet to all the cuts. But, unless you can find stock ones, getting them custom-radiused is not cheap. I get charged $18 per endmill to add a radius...but I use really nice ones from SwiftCarb that already cost $50-$100 each, so increasing the tool life by 5x or more is well worth that cost.

6) Extended length, reduced-shank bits. When needing to dig really deep holes, like a 2" hole through a block of aluminum, our Sharks can't handle an entire 2" of engagement on the flutes: it pulls the head down into the hole in horrible ways. But, with these, the cutting flutes are only about 0.3-0.5" long; above the cutting flutes is a reduced-diameter shank that gives that extended reach, without touching the hole sides (when the spindle is properly aligned). Of course, when one bit costs $80, adding another $18 for custom radiusing is nothing, when it increases tool life by 5x or more. One tiny nick in those sharp tips is all it takes to make an endmill worthless, leaving scratch marks on the vertical walls and pocket floors.

7) High-speed steel tooling. Interestingly, HSS sharpens sharper than carbide. That is, a proper HSS edge is actually sharper than the more-brittle solid carbide cutting edge. And, when run at the proper F&S, HSS can actually last LONGER than carbide. I'd say give them a try. At 1/4-1/3 the cost per cutting edge, sometimes it makes sense. I use them in O-flute (aka 1-flute) standard sizes and nominal lengths for acrylic and wood, and they do indeed stay sharp longer than a similar carbide bit treated the same way. These guys are so cheap, you can often buy them in multi-packs too.

8) Flatification tools: these are the fly-cutters and the larger-diameter end mills, and are used to create large flat surfaces. I use an HSS 0.75" diameter stub end mill that's normally used in an old Bridgeport mill. They're about the largest diameter cutter I was able to get to work properly in aluminum. Wood can likely take the larger, say 2" diameter, 4 carbide-insert fly cutters.

9) Spring-loaded, split-blank engraving tools. If you need to engrave (really!) small text, you'll eventually find your way to using 1/8" shank, 15- or 30-degree included angle engraving bits. These have "one" flute where they have ground off half the tool's diameter. When you get down to final tip-diameters in the 0.005" range, a bunch of unexpected effects occur. The first is that you really can't dig very deeply with them, especially into metal. 0.002"-0.003" maximum depth-of-cut is not uncommon. But, the surface-height variation of nearly all materials, unless they're precision-ground and registered in the CNC machine, is more than 0.003", often by an order of magnitude. Which means that if you want to have a consistent-width line, it's not "height" but the "pressure" that needs to be consistent. It's the pressure that really determines how far into the material the bit goes. Thus the adjustable spring-loaded engraving bit holders, that run from about $80 and up, depending on complexity and quality. The bits that go in them are cheap cheap cheap, often well under $1 each, IIRC. I've had great success engraving letterforms down to about 0.030" total height using one of those. The second thing to deal with is some scamming on the part of eBay sellers of the engraving bits. Sometimes they claim 30 degress with a 0.005" tip. But, on very close examination, what you find is that indeed, the tip is 0.005" across..but for the first 0.010" vertically, it's NOT 30-degrees, but is more like 120-degrees. Which means that you're not ever really going to get an 0.005" tip diameter, because at any real cutting depth, the line-width changes like a 120-degree bit. So, you get 30-degrees, but only for lines in the 0.015" and over depth range...which takes multiple cuts to get that deep...tiny text is a difficult thing :D. One final obscure note with these is that the spring-loaded holders very often have RPM limitations, which will directly affect the cut quality because that defines the SFM. In some metals that can make finding a viable cutting solution very difficult.

10) Spot-drill and center-drilling bits are useful when you want to precisely locate a hole relative to the rest of the machining, but the actual hole-drilling will occur off the CNC.

11) Chamfer and round-over bits. These tend to be difficult to properly place, because the flat chamfered face will change in width as the precise alignment varies around the perimeter of whatever you're chamfering. But, if you can get them aligned properly, breaking those sharp edges can be very beneficial. That's especially true when the profile is complex and difficult and time-consuming to deburr/defuzz manually, and you need to make a lot of the parts. Chamfer bits can also be used to create countersinks for flat-headed screws. Just remember that US countersinks are 82 degrees, while metric countersinks are 90 degrees. Using a 90-degree chamfer bit to create a US countersink (especially in metal) is a recipe for bolts that don't stay tight or hold very well. Also, remember that the bolt's connection to the conical-section of the flat-head is radiused: if you don't break the edge at the bottom of the chamfer feature in your part, and the hole clearance is minimal, it can score the bolt and weaken it. (How's THAT for obscure?)

12) Specialized bits: If you are REALLY confident in your toolpath generation ability, either through software or custom, you can try things like a dovetailing bit, or other cool ones like an o-ring holding groove. The bit profiles and functions aren't that difficult to understand, but getting the lead-in and lead-out correct on those is an absolute, non-negotiable requirement. If you can't get the leads right, might as well not even bother trying, because the bit is going to be destroyed on its first use, and you will cry. I know I did!

13) Tapping. While loosely related, it's an important thing for me. Since I do a lot of aluminum parts that have to be put together to make a rigid assembly, this design choice comes up every day: either put in some nice threads directly into the part, or figure out a way to have nuts and bolts everywhere. I chose the first, and picked up a couple TapMatic heads that go into my drill press. In about 1.5 seconds per hole, I can tap anything from #0000 to 1/2", with almost no chance of breaking the tap in the material. They're wonderful devices, and thankfully can be found on eBay used: they're tanks that last forever. This, of course, opens up a whole 'nother world of buying different taps: long ones, short ones, thread-forming and thread-cutting taps, course, fine and NPT threads, and the exact drill-sizes for them to get just the right thread engagement. That's right, I can now create threads that effectively form their own lockwasher/shakeproof fastener and have ultimate pull-out strengths rivaling any other industrial tapping method :D

14) Alternative cutting technologies: yeah, we're talking LASERs here :D. In their various forms, they're just another cutting/marking tool, right?

15) One I haven't tried yet, but want to, is to chuck a 1/2" diameter wire brush (1/8" shank) into the spindle, run it at really low speeds of say 500 RPM, and use that to apply a finish to a (metal) part. The brush would be like a small, dremel-tool cup-shaped wire brush, and the amount of pressure applied would be very little. I've heard good things about it being able to hide other machining marks and give a cool "jeweled" surface texture. Extra points for "dabbing" the brush down to make a tiled-circles pattern.

One overarching piece of advice I'll give, but few seem to agree in practice: never start a cut unless you already have the "next" bit for that cut on hand. That is, always keep a spare, new bit on hand, and order in that one's replacement when you start to use it. Bits, especially delicate ones, break, and get dull. They don't last forever. So, if I'm planning on cutting something, and I notice my cut-plan says to use a bit I have only one of, well, I start getting nervous. If something goes wrong, and the bit breaks, first there's the issue of whether I'll choose to wait for shipping to get the bit(s), or I'll take the chance a local source will be open and has them in stock. Then, the real issue arises: if I've already started a cut, and the bit breaks, and I don't have another bit to finish it with, I can't move on to a different project without giving up my work-holding arrangement and alignment, as well as losing the part registration for that cut. Heck, I can't even move forward in THAT project. Which essentially means another choice: either that part is now in most cases waste, or the machine sits idle until I can get a new bit to finish the cut. By always having the "next" bit on hand (and yes, that next bit's next bit too ;-) ), I know I'll at least be able to recover from ONE major error if needed, and if the errors are small, chances are I can get it to run right and not use the next bit.

That's about as far as I've gotten. There are some bizarre and amazing bits out there, like reaming bars and tapping heads, none of which are really useful for us to use on the CNC, just due to the overall capabilities of the machine. But, the sky's the limit elsewhere. All it takes is moolah. :D

Regards,

Thom
Last edited by Rando on Mon Dec 04, 2017 7:39 pm, edited 9 times in total.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 462
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA

Re: Bits to purchase next

Postby Kayvon » Mon Dec 04, 2017 6:38 pm

Great, detailed advice, Thom.
Rando wrote:our Sharks can't handle an entire 2" of engagement on the flutes: it pulls the head down into the hole in horrible ways.
That hurts just reading it.
User avatar
Kayvon
 
Posts: 271
Joined: Tue Oct 21, 2014 11:46 pm


Return to CNC Shark

Who is online

Users browsing this forum: No registered users and 5 guests

cron