View Full Version : Large VCarve Problems

05-30-2009, 12:30 PM
I am a bit of a newbie on this... especially doing something on the size scale of these letters.

As you can see below the scale of this logo is fairly large (by my standards)at 18" in length.

This is being cut into the back of a solid Maple cutting board that I made. The issue is that i am seeing lots of material left and the letters are very very rough as you see in the 2nd and 3rd photo.

Another issue that I have that I have never seen are the noticable burn marks being left by the tool as it changes directions.

I am using a Centurion 120deg 1/4" Vcarve bit. This is the first time I have cut with a 120 so there may be something here I am missing. (VERY LIKELY)

My bot is a 48" Buddy with spindle

The parameters I last tried were:

Included angle = 120
Pass Depth = 0.06
Final Pass Stepover = 0.025
Clearance Pass Stepover = 0.025

Spindle speed = 14K

Feed rate = 3
Plunge rate =1

Any thoughts, ideas? Please don't say sand!

Thanks everyone!

Ken Brown




05-30-2009, 05:25 PM

I'd recommend getting a larger diameter 120 bit first (I have a 1.75" diameter one that works well for larger designs). As you can see, the tool has to step down 5 times to get to the final depth and that can cause the waterline marks. The bit geometry may be off a little, although the Centurion bits are generally right on.

It looks like there may be some overlapping vectors in your design or some inside of another on the smoke tail which will cause it to carve inside each closed area. Do you have "Flat Bottom" checked? Final pass to large?

While I love using Centurion's v-bits for carving veneered MDF, I find that I can't use them in solid wood. Their cutting action is more like a scraper and causes tearout in maple and cherry along with burning. You may want to slow the rpm's down a bit. I'm usally around 12000 +/-.

For solid wood I like a good two flute v-bit. I've had good luck with these (http://allita.net/Projects/omnicat5/ShowItem.php?cat_id=0&sku=615-690) 0.5" shank 0.75" diameter 90 bits. From here (http://allita.net/Projects/omnicat5/index.php?cat_id=0) or here (http://www.infinitytools.com/products.asp?dept=1057) for a decent price.

05-31-2009, 12:47 AM
Thanks Scott!

As I was out running errands this afternoon I could not stop thinking about this situation and had concluded that the small bit vs the large letters were likely my issue... thanks for the suggestions and links!

Now I need to try to get a larger 120 and try to clean up this piece...

Thanks much again!

05-31-2009, 01:14 AM
Many tools might be off by a degree or two because they are cheap imports. I have seen the tools under a special instrument measured to be EXACTLY what they are supposed to be from centurion so you might try them.

05-31-2009, 11:43 AM
Take a look at Hersaf indexable v bits. Get a big enough bit you can vcarve to depth in a single pass.

06-01-2009, 06:31 AM

I'll echo what Scott said. I cut hardwoods almost exclusively, and I have found that the Centurion V bits are not the best for this application. Don't get me wrong, though - Centurion makes excellent bits, and their V bits do a terrific job on MDF, HDU, and other composite materials.

The burning is caused by too slow a feed rate, RPM's that are too high, a dull bit, or a combination of the above factors. Hard woods like maple will burn easier, and require some tweaking of feedrates and RPM's to optimize the cut.

I have had good results with V bits from Whiteside, Amana, Onsrud, and Magnate.

The need for a large enough bit to do the carving in a single pass cannot be overstated.

Finally, the type of hardwood is important as well. Maple and other dense, close grained species do the best. Softer woods like cedar, cypress, etc. tend to have more tear out and roughness. A very sharp bit and extensive experimentation can minimize this.

Hope this helps.


06-02-2009, 01:03 AM
Again to everyone ... THANKS!

I ordered some V bits from Onsrud.. I have been using the Centurion bits exclusively and this was my firt try with their 1/4" 120...

Thanks Matt for the suggestions too on the feed rate and RPM's....


06-02-2009, 09:14 PM
Well might as well toss out my experience as well. I am by no means well versed in V-carving, however, I used the 1" 60 degree Onsrud that is in the selection ShopBot offers on one of my first lettering jobs. The material was American Cherry and the result was poor at best with significant attached slivers of material remaining in the grooves and noticable tearout. The RPMs were 16K, depth 0.10" and speed 1.5"/sec. Trial cuts looked great in MDF so I thought I was home free. One major lesson learned - "run trial cuts in same material". After consulting with another "experienced" local ShopBotter, I followed his advice and re-did the job using a 60 degree CMT Lazer point (858.501.11). Result was exceptionally clean and crisp.

06-03-2009, 06:07 PM
I have only been shopbotting for a little over a year and have used Centurion V bits exclusively. I haven't had a problem using them in hardwood. I have V carved oak, cherry, walnut, hard maple, and cedar. All have turned out great. I use a PC router and run my bits at 19000 rpm even on the 120 V-bit. As someone suggested, I would definitely move up to the 1/2" version.

ron brown
06-05-2009, 05:55 PM
I'm with Ken on Her-Saf bits. I like mine and there is not a less expensive bit for production runs.


06-06-2009, 01:23 AM
I have been happy with the 60 and the 45 centurion vcarve bits. but for solid woods you need to slow them down. the 120 I have never used that one.

06-13-2009, 08:21 PM
Another option might be looking at a place that sells machine shop supplies. They have bits with replaceable carbide cuters. I use 1 from my mill, it's expensive but good cutters make a big difference. One other thing, make sure your using a high quality collet and things are clean before you tighten things down.

06-14-2009, 12:54 AM
Ron, I just got one of the Her-Saf V90 cutters, but haven't had time to try it out yet. I was wondering what rpm have found that works good with these since they are a single edge cutter? Have you found that the inserts last the same as standard carbide bits? I've got a repeat job that the larger diameter V90 should save me some time and clean-up (I hope).

ron brown
06-14-2009, 08:28 AM
"Have you found that the inserts last the same as standard carbide bits?"

Well, in a word, no. I've found the insert bits from Her_Saf last a lot longer than the brazed on bits. I had one project where I was able to actually run parts with a 1/2" insert bit in a production job. It went over 6,000 LF in maple.

It does stand reasoning that a screw held insert can be treated differently than one that is brazed then sharpened.