Need Some V-Carve Advice

[Burkhardt]

I have not used my machine for V-carving much but tried a couple of things lately. But, like mentioned by somebody else in the recent "messy steps" thread the results vary. I did a comparison test today with several 60-degree bits I had around. Please see the bit description below. All cuts were made in Con Heart redwood, which cuts cleanly but is a bit sensitive to tear-out. Feed rate 80 ipm (1.33 ips) at 14,000 rpm and 0.2" depth steps. Obviously the Amana blade has by far the best result in spite (or maybe because) of the broken tip. I would appreciate an opinion on the results and other suggestions. I know, e.g. the Whiteside bits are quite popular but I did not have one to test. All cuts are as they come from the machine, no sanding.

The Good: Amana In-Groove. Quite new but I ruined the tip when I tried to run it in maple at 120 ipm. Has only one cutting edge but can not run much faster than 15,000 rpm on my machine due to unbalance.
https://lh4.googleusercontent.com/-ZJrrtbBuRCg/UtNRreFdJNI/AAAAAAAAEgI/Gt1LFGbWwSQ/w647-h862-no/DSC02135.JPG

Still O.K.: new 2-flute Kyocera engraving bit 1/4". Very sharp but the tip leaves some depth step. It is only a few 1/1000", barely perceptible with the fingernail but still quite visible.
https://lh4.googleusercontent.com/-5EPaxdPn9-g/UtNRtdcNrYI/AAAAAAAAEgQ/diScN5XhKSw/w647-h862-no/DSC02136.JPG

The Bad: same Kyocera bit but I thought to "improve" the tip with a diamond hone.....much more tear-out. Maybe I should just blunt the tip completely (like the Amana)
https://lh6.googleusercontent.com/-8RP8YgjwVFg/UtNRvS0vTuI/AAAAAAAAEgY/gkHud4f4wlQ/w647-h862-no/DSC02137.JPG

And the Ugly: 1.25" V-bit from some eBay seller. I have used this bit already for several jobs and mostly the result looks better.
https://lh5.googleusercontent.com/-jjES8_fRC5s/UtNRxBj3E9I/AAAAAAAAEgg/x6zFUqw1O6c/w647-h862-no/DSC02138.JPG

[myxpykalix]

you might want to check out centuriontools. I've been using mine for several years and they stay sharp.

[steve_g]

Gert…
I’m happiest with the CMT 3 flute laser point bit…

SG

[scottp55]

G., I only do teeny stuff, but the deepest cut in this pic is .37" and the step on the bit is only .06 (.1245 60degree) and that cut is still on the table untouched. Funny it isn't even a vbit- its a 60 degree SC countersink with a .005" flat. Your broken amana was the best by far-I'd lose the Kyocera. Oh. cherry 1.2,.5,13K. Hope other people chime in on 1/4" 60's with pics

[Brady Watson]

I've only had precise results from Gerber and Amana insert bits (not in-groove). They are the only large diameter bits with properly ground angles that I have found over the years. Neither are cheap, but then again you see what you get with bits like the Ebay cheapie.

With any insert bit you have to be very conservative with stepdown. I wasted a 45 deg Amana in maple when the insert got yanked out of the holder and now it is completely junk...apparently they are not designed to cut maple 1/2" deep in one go...total brainfart...it happens to the best of us some days.

ANY v-shaped tool scrapes at the very point. Knocking off the tip will help cutting, but you won't get sharp prismatic corners and features that v-carving is known for. When v-carving is done properly, you should be able to stand back from it looking dead on & not be able to tell if it is prismatic or incised. It grabs your attention and makes you look twice.

If you are getting step down marks in your v-carving, it is telling you that your tool diameter is too small. You are going to get some lines anytime you have a stepdown in the finish surface. A large dia tool that can do the cleanup pass in one go will not show these lines. I have Gerber and Freud v-bits up to 2" in dia. These are mostly for HDU signs, but on occasion a 2" 90 is nice for doing 45s on dimensional lumber and other things.

The smaller bits already mentioned are great for smaller letters and designs, but once you start to carve larger designs and letters, you need larger diameter tools to get the quality of cut you are after.

-B

[chubb]

Hi G.,

If i'm doing V-carve (chipcarving) work with a tool that cannot complete the design in one pass I always grind the tip to a radius ball point between 1mm-2mm diameter. The greater the radius of the rounded tip the less obvious the stepping is. The only draw-back to that is that the greater the radius the less sharp your corner edges will be. Depending on the scale of the pattern, I would decide on the maximum tip radius that would still give relatively good 'chipcarved' looking work. The larger the work the less perceptible unsharp corners are. I find that you can only tell that a corner isn't sharp if you use a 1.5mm diameter and look really close.

My rule of thumb is:

work with elements less than 10mm - usually done in one pass
work with elements 10-20mm - ~1mm diameter
work with elements 20-35mm - ~1.5mm diameter
work with elements 35mm and larger - 2mm diameter

I'll sometimes change these values depending on the angle of the bit and the hardness of the wood.

For really large work I'll just use my 1" Onsrud 60deg tool that I ground the tip to a 1mm Diameter.

Using these I find that it leaves a super clean edge that requires no further sanding. I'm suspecting you're still getting lines per pass coz the flat tip still has a sharp edge rather than a rounded edge.



Some further tips I follow-

-Use the hardest timber available (holds a better edge and less prone to chipping and splintering

- if you can do a cut in one pass - use a conservative plunge rate and feedrate (more conservative for harder wood)

- try not to let two vcut overlap (you could get chipping off the top edge that ends up looking horrible). I try to leave a 0.5-1mm gap at the top. Looks like you've done the same in your photos.

- use a cutter whose cutter geometry is centred. i.e. if you look at the top of the cutter, the cutting edges on opposing sides (or all cutter edges if using one with more than two flutes) must meet dead centre, and not be offset from the true centre (learned this one from you on the 'messy v-groove' thread ;) ). These kinds of cutters are usually the 'carbide tipped' type, you unfortunately can't correct this issue by grinding. I would only use these tools for single pass work.

- use a sharp cutter :)

- try as much as possible to do all cuts in one pass.


Hope the info helps.

Done alot of v-groove cutting and learnt some of the above the hard way.

Mark

[Burkhardt]

Thanks guys, great information!

I will order the CMT bit for comparison and maybe the Whiteside, too and keep experimenting, also with rounding of the anyway broken tip. The big Amana insert bit is a bit "rich" for me at this time :rolleyes:

Did anybody try a roughing/finishing method with a very big bit? That would be doing a first high speed removal of the bulk material in reasonable depth steps running the path maybe 20 or 40/1000" high and then a single slower pass at full depth and correct starting level to skim the depth marks and create the final shape.

[Brady Watson]

That's a 'trick' that many of us have done - drop the Z down .01 deeper and clean it up in one go.

-B

[supertigre]

From the steps on the side of the carving it looks like only the Amana is actually 60 degrees, everything else is not.

[Chuck Keysor]

Hello Gert. Thanks for publishing the side by side comparison photos. I always find such evaluations to be very enlightening, and I think they are a great public service.

First, let me say that I too purchased the Amana "In-Groove" tool, as part of their 8 piece packaged set. And like you, I too had my tip break off really fast, while I was still cutting the first piece, which was only MDF, at 1.5IPS, and it was a shallow cut making small letters. Before breaking, the grooves were awesome! After breaking, just as in your case, the side walls were still beautiful (no real consolation though, as I wanted a sharp bottom in my grooves:mad:). That set came with 4 sharply pointed tips. All broke with almost no use, only cutting MDF. (I did call Txxxx Txxxx, where I bought these and complained, and they referred me to Amana's tech support, and after one try of being on hold, I simply didn't bother again:() I figure it is best to let people know about these bad tools, so that they can either avoid buying them, or at least not feel like they are stupid and have messed something up by doing something dumb.

I too had some other cheapie conventional V bits I had purchased brand new, and I too had poor results, in poor bottom of groove definition, but not with the sidewalls, because my cuts were so shallow (again, just small letters, then some art type engravings), I did them in one pass. But when I complained on this forum, and asked for suggestions, the CMT Laser point bits were recommended by a couple of people, perhaps Steve G. was one of them. But I have had great success using 60 degree three wing CMT Laser bits.


I look forward to your future pictures showing how well your CMT Laser bit works. Good luck, Chuck

[danhamm]

Just did a little carving with a Kyocera .25 60 degree v bit its on light mdf spray painted. 4 inches sq.

thats a toonie up in corner.

[scottp55]

That came out Nice Dan! One pass? Depth of cut?

[danhamm]

no depth set, used vcarvepro yes one pass.

[Burkhardt]

Just did a little carving with a Kyocera .25 60 degree v bit its on light mdf spray painted. 4 inches sq.

thats a toonie up in corner.

Very nice indeed. The kyocera bits are great if you can cut in one pass. They are economic, too.

I guess Brady is right about the tip of any sharp v-bit just scraping or dragging because even at high rpm the circumferential or surface velocity is very small. Add the imperfections of the bit grind and it will leave a trace that may get worse the sharper the tip is. In that case the options seem to be:
- do a single pass if possible. For deep cuts it will need a very large bit and big spindle or low feed
- use a slightly blunt tip bit if the rounded groove bottom is acceptable
- do two cuts as mentioned in the other post with a large bit. 1st to remove bulk in layers and 2nd single pass to finish/clean up a little lower
- do two passes with a blunt bit first to remove the bulk without step trace then a finish pass with a sharp bit to clean out the bottom. Setting the proper z-height for the 2nd pass to match the first one will be a challenge, though.

I will still try how the CMT and Whiteside bits are behaving in multi-layer cuts. Quite interesting and I am still learning.

[Brady Watson]

If you look at the geometry of an engraving bit, you'll see that the tip is offset at least .005; although .015" seems to be the norm. I like the Micro100 stuff, which works pretty well on fine shallow engravings and things like PhotoVCarve etc.

-B

[Burkhardt]

I am getting there...did some more tests (increased rpm to 18,000 for both trials):

1. roughing cut with blunted 0.25" Kyocera bit in layers at 1.25ips and 0.125" depth step. This bit is lopped off straight 55/1000" at the tip. It leaves very minimal layer or depth step traces. These are really not steps or grooves anymore but a fine line in the wood. I have not tried actually rounding the tip, though.
2. Finish cut with an unmodified Kyocera bit. The tool path was created for a huge 2" diameter bit at full depth so that this cut only scrapes out the bottom of the groove very cleanly. Turns out the matching depth setting was very easy because I can measure the length of both bits with a caliper. The unmodified bit is exactly 2.500" long while the shortened bit is 55/1000" shorter.

Surface quality is very good. Almost no tear-out and very smooth which means something for such material:
https://lh4.googleusercontent.com/-SzbSdAjHLaA/UtSsB99m97I/AAAAAAAAEgw/lv3mEZi5GQE/w647-h862-no/DSC02139.JPG


Both cuts with the cheap eBay bit 1.25" diameter 60 degree, unmodified.

1. rough cut 80/1000" high to leave a skin in 0.25" layers at 1.25ips. As expected this makes some pretty bad depth step lines.

2. finish cut with same bit at nominal height for a single pass at full depth. I had to reduce the feed rate to 0.6ips to avoid ripping off some of the intricate edges. But that single pass is anyway rather quick and the low speed is O.K.

The result is actually quite nice. No depth lines whatsoever, the 80 mil from roughing to finish take care of that. Surface is not quite as good as with the Kyocera bit but for me very acceptable and the bottom edge not quite as sharp. But, I think it can be used for most of what I need to do and in good quality hardwood the result may even be better.

https://lh6.googleusercontent.com/-B7DnS03Yo8o/UtSsDXCORNI/AAAAAAAAEg4/8FPBtgMLVW8/w647-h862-no/DSC02140.JPG

[chubb]

Hi Burkhardt,

That looks like some significant improvement on both bit types. But the ebay bit is quite impressive with how dramatic the change is.

looks like doing a clearance pass then a finish pass dramatically raises the quality.

Real good info in this thread.

Thanks for updating. Really good photos and comparison.


Mark

[Brady Watson]

How much meat did you leave on it before you did the cleanup pass? I usually do like .030 by Zzeroing high, then lower the Z down to true 0 and run it full depth for the final clean up.

-B

[Burkhardt]

How much meat did you leave on it before you did the cleanup pass? I usually do like .030 by Zzeroing high, then lower the Z down to true 0 and run it full depth for the final clean up.

-B

That is what I tried first. But the cheap bit leaves some pretty nasty gashes and 0.03 was not enough to remove these traces. So I used 0.08" which may be a little excessive but it did the job. Keep in mind the redwood is soft but very brittle.

I was wondering also about the rigidity of my machine having an influence on such steps since the accuracy with the small bit is somewhat better. Obviously not a Shopbot but at 6000 lbs/in in x-direction and 3000 lbs/in in y direction (measured "scientifically" with a dial indicator and a fishing scale) and about +/- 0.0016" backlash I had hoped it should be good enough for this kind of work.

[scottp55]

G., You may not be a Shopbotter, but stuff like this helps everybody and is very informative. Dramatic improvement and pics and #'s helped show the progression of the "blended" techniques. Good toolpathing stuff and alternatives. (should have asked "pass depth" setting in database) Good work Gert.

[shilala]

I just wanted to kick in my 2 cents.
The only v-carve bit I have is a 1" 60* 1/2" shank 37-82 Onsrud. It's never cut anything but perfect v-carves, no matter the depth. I do cut very shallow passes, though.
I's like a 90* bit, and when I finally get one, I'll get an Onsrud just because the 60* has done so well.
I just realized that this is probably the one problem I've seen here that I've not had.
It had to happen sooner or later. :D

[ssflyer]

I use the same Onsrud bit, and their 90 Degree 37-87 1 1/2" bits. They work great for me, and I don't take shallow cuts. :)

[Burkhardt]

I use the same Onsrud bit, and their 90 Degree 37-87 1 1/2" bits. They work great for me, and I don't take shallow cuts. :)

I wonder if Onsrud has a trick to grinding the tip so that it leaves no trace (maybe the CMT guys have one too but I did not get the ordered bit yet).

So if you v-carve deep with several depth steps you do not get any witness lines for the depth steps? What feed rate do you use?

For what it is worth...the maximum groove depth of my sample parts is 1.3"

[RossMosh]

My limited experience is that I haven't liked my Magnate bits at all. They seem to love to break at the tip. I wouldn't recommend them at all. I have a Freud 90* bit that gives good results but it does not come to a sharp tip. If you're okay with a slightly blunted tip, the Freud bit isn't bad.

[pappybaynes]

[QUOTE=bradywatson;158203]I've only had precise results from Gerber and Amana insert bits (not in-groove). Gerber??? where do you find those Brady??
thanks Dick

[Brady Watson]

Dick,
You can get them from Gerber Scientific (http://www.gspinc.com/default.asp?contentID=253), among other places. In case you didn't know..."G-Code" = "Gerber Code" - they pretty much invented it.

-B

[Burkhardt]

More experiments....I hope nobody is going to accuse me of getting a bit anal about that.

Anyway I did get the CMT laser point 3-flute bit. Quite different, as they don't use carbide plate inserts but instead a carbide plug in a steel retainer and grind the whole thing together. Very sharp tip and reasonable surface quality but unlike all the other bits, the tip creates not just a groove/score but a real step. I am going to take it to work tomorrow and measure the flute angle on the optical projection comparator. Result is a somewhat disappointing, at least not better than e.g. the Kyocera bit.
https://lh3.googleusercontent.com/-wZIwm8Pq1X0/UtYYC9rv6hI/AAAAAAAAEhM/lZVbOTRk5Ww/w647-h862-no/DSC02143.JPG

I repeated the test with the blunted Kyocera bit but tried to give the bit tip some radius. After that I cut the groove bottom with the CMT bit (probably could have used any other sharp tip bit as well. The result is slightly better than with the straight blunted bit but still some lines left to see.
https://lh5.googleusercontent.com/-LZiiJFR_Y4I/UtYYE72RWEI/AAAAAAAAEhU/jDfLCK2GOf4/w647-h862-no/DSC02144.JPG

Finally I tried to do a rough cut with a blunt radiused tip bit (the small one) that I had for a while, no idea what brand. That left minor step lines and I finish cut with the large 1.25" eBay bit. I would say that gave me the best result except some tear-out from the roughing path (I guess the bit is not that sharp anymore).
https://lh5.googleusercontent.com/-tL_Se3An_aA/UtYYG775h0I/AAAAAAAAEhc/8vLKTvomrvg/w647-h862-no/DSC02145.JPG

[Burkhardt]

Given the mixed results from my test and some members here posting that it should not be a problem at all I would like to propose a challenge...

Please take the attached V-Carve file and cut the pattern into redwood or comparable lumber (I used 2x6 kiln dried ConHeart deck boards), take a picture and then let me know the secret: bit type, speed, feed, depth etc.

I would really appreciate it! G.B.

[steve_g]

Your test results make me wonder if individual bits of a manufacturer vary considerably…
SG

[myxpykalix]

G,
I think you really need to check out centuriontools.com see the pic i posted on page 1 of this thread and you will see very pointy sharp bits. They showed me on some machine (don't recall what it was named), where they had angle deliniations and you stuck the bit in and it showed you that it was a perfect angle. If you look at the 120 degree bit, that one has made me bleed more times then i can recall.:eek:

[scottp55]

Gert, just to warn people, .crv as shown with 60vbit will cut into table. Max depth as shown is 1.663".

[Burkhardt]

Gert, just to warn people, .crv as shown with 60vbit will cut into table. Max depth as shown is 1.663".

Thanks for the warning...But I had set the flat depth to 1.3" which should leave 0.2" residual wall in a 1.5" thick stud. Did the "flat" check mark get lost?

[scottp55]

Sorry G., No it was there on all your bits, just didn't show up when I inserted my bit from database, never watched/checked your toolpaths. Had to half scale your design as no thick cedar or torrefied to play with, and don't have .25" 60vbit(or the time with an .125" 60vbit for that matter). It won't be a real comparison for your "challenge" but at half scale everything should be similar enough to satisfy my curiosity.

[Burkhardt]

G,
I think you really need to check out centuriontools.com .... I have one of their 90-degree pyramidal engravers but did not use it much. Maybe I try to get a 60 degree bit for comparison with the others.

Today I got the highly acclaimed (on other forums posts) Whiteside bit but man, what a disappointment:

https://lh5.googleusercontent.com/-00O_FOLX5e0/UtdX3T82n-I/AAAAAAAAEhs/gxJIJJvUyGk/w830-h862-no/DSC02147.JPG

Since I had some reasonable results so far with the large 1.25" bit (actually I looked it up I bought it from Amazon for $8.99 each (http://www.amazon.com/gp/product/B00HDAH882), not eBay). I free-hand modified one of them with a small radius at the tip and did the rough cut 0.045" high to compensate for the radiused tip plus 0.015" to leave a skin. Going 0.25" per depth layer left very minor depth traces and I could probably have gone 0.3 or 0.4" deep just as well. Speed 14,000rpm and 1.25ips.

Then I did the finish cut with the same bit but unmodified tip in a single pass. Speed 14,000 rpm and 0.66ips. I am very pleased with the results. The surface is pretty much ready to laquer, the small depth lines machined away and very little tear-out or damage to the slim surface ridge. I think I found the optimal combination for this material. I will try it in hardwood sometimes, too.

https://lh5.googleusercontent.com/-sdPLopTPGc8/UtdX57uF-eI/AAAAAAAAEh0/bCpPkWv_qxU/w831-h862-no/DSC02148.JPG

My wife asked me already what I was planning to do with all the cookie molds...

[scottp55]

G., not a true test as it's half scale(had to add a .01" circle in center so it wouldn't cut into my first 3D on back of scrap) ,but cut with an 1/8" 60vbit. Wish I hadn't use flat grained stock as the the growth rings look like tool marks,BUT they aren't. Wood is C-90 Torrefied ash and the chips on the top are only because the pores are so large it's like a brittle sponge. Zero sanding but you don't have that "crispness" Brady was talking about. But we're doing(or will be doing) 144 kids alphabet blocks,6 sides 2 batches a day and the lack of sanding is worth it.That was fun! Can we safely use that file(without copyright problems). Or would you rather we don't. http://www.carbideplus.com/Carbide_60_deg_3F_Countersink_p/333-001050.htm

[scottp55]

No finish, just the flash bounce. straight off/on machine.

[Burkhardt]

.... Can we safely use that file(without copyright problems). Or would you rather we don't. .... No problem using that file any way you like. I created that on the fly for the specific purpose of bit testing.

What feed and speed did you use and how deep at one depth step?

Thanks for testing! Today I found v-groove bit from MLCS that comes already with a 0.02 radiused tip (#7718 on this page (http://www.mlcswoodworking.com/shopsite_sc/store/html/smarthtml/pages/bt_sign.html)). I will try that, too.

[scottp55]

1.2,.5,13K .07 pass depth. for maple go .06" Had a little deflection as had bit exposed 7/8" could have gone shorter. Good chips bit cool.

[scottp55]

Oh I tried that same bit in a 90 and the flat was about .02 and it was way to much flat for an 1/8" Thought my 60 was a fluke at .005 flat, but bought another 8 and they are all identical. That bit I used has about 12 hours of maple vcarving on it ,so I used it as I'd never gone that deep with it. New ones better.

[chubb]

https://lh5.googleusercontent.com/-sdPLopTPGc8/UtdX57uF-eI/AAAAAAAAEh0/bCpPkWv_qxU/w831-h862-no/DSC02148.JPG

My wife asked me already what I was planning to do with all the cookie molds...

That, sir, is a very pretty cut :cool:

It really looks absolutely brilliant.