Carving Photographs and Breaking Bits

[daniel]

Hey Guys, here is a pic of Ray Charles I cut out.
Looks great but the bits I use tend to break off at the tip. They are much bigger bits than I need, There 45 degree 5/8 diameter. Is there any 45 degree bits out there that are stronger and made just for engraving?

6312

[daniel]

Here is the bit I am currently using, Its a little blurry, but the tips keep breaking off.

6313

[scottcox]

Daniel,

That looks great!

Can you explain to us new guys how you did that? Which software/converter/techniques did you use?

[paco]

Hey Daniel!

You might want to look for half round engraving bits...


Examples

6314 (http://www.bitsbits.net/images/tlet_half_round.jpg)
http://www.bitsbits.net/index.php?main_page=index&cPath=3&zenid=baab7834e4 9235a516c2bc22ba9a92cc

This is pretty pointy and you might want tipped off types(0.005-0.03").

Onsrud have a serie with 1/4" shank. 37-00/37-20

[patricktoomey]

Daniel, I do a fair amount of carving with 45 degree V bits in wood and Corian. They eventually go dull but I've never seen a tip break off like that except when a grounding problem caused my spindle to plant one half way through my aluminum Z zero plate. Are you using HSS bits, carbide tipped or solid carbide? Also, what is your feed rate, RPM and depth of cut? I'm wondering if the bit is overheating due to excessive RPM.

[drodda]

I had the exact same problem with the bit breaking off on my 45 degree bits. I have purchase the conical engraving bits but have not had a chance to give them a try. I thought it was something that I messed up. Maybe not?

Dave

[burchbot]

Hi Scott
I believe the program he is using is Photo V Carve by Vectric. You can download a trial version of the program at the Vectric website. While you are there be sure and check out V Carve Pro. The Vectric forum is a great place for information too.
Dan
6315

[phil_o]

I had a problem breaking the points on 60 degree V-bits. It always happened when i used the Z-zero plate to zero the Z axis. Now I use the keyboard control to slowly jog the cutter down to a piece of paper on the cutting material. Once the point of the cutter grabs the paper I zero Z with the "Z Z" command. Hope this helps.

[beacon14]

I think it's a good idea in general to reduce the Z move speeds in the z-zero program. The Z moves as written in my opinion are way too fast for delicate carbide bit tips - even a more substantial tip on a larger bit has a delicate point and will chip when rammed into what is effectively a metal table.

[tony_mac]

Tip for PhotoVCarve users that should help prevent the tips being broken off the cutters.

PhotoVCarve has a special roughing strategy that will carve using multiple Z Level passes, but only where they are needed.

This option is initiated by setting the Pass Depth for the cutter to be less than the Carving Max Depth.

For example, if the Carving Max Depth is set to 0.060", then setting the Pass Depth for the cutter to be 0.030" will result in 2 Z passes. But NOT for the complete job, only in the deeper (typically darker) regions of the photograph.

I hope this helps,

Tony

[daniel]

Hey Guys,
The cutfile for the ray picture was done in ArtCam, The V-bit I was using is a carbide tip not a solid carbide bit. It looked fragile.

I have a hard time sanding and finishing wood in my tiny little space, so I brought some 3/4" thick hard wood flooring that was already finished beautfully. It was also tounge and grooved. I just glued up three pieces then ran the cut file, put stain all over it and wiped it off.

Paco, Thanks for the link, I just ordered an onsrud 30 degree engraving bit, I bet its going to work Great!.

Thanks again Guys!

[daniel]

Oh yeah, Patrick
The feed rate was 1.7 inch/min
The max depth of cut was .15 inches
And I have no idea what the spindle speed was, whatever rpm that 3 represents on a 2 1/4hp makita router.

[workingdog]

Daniel,
Can you tell us a little more about how you did the ray picture in ArtCam?

[daniel]

We created a model from an image(picture). We sized it to 16" by, I think 22". The hieght of the model created was set at .15". Then we went to toolpaths and selected "machine relief", we chose a 45 degree v-bit and set the step over at .0115". And we also used a 45degree raster machine strategy. Thats it!

I must say it takes a little trial and error. So far I'm 2 and 2. I've made two that look great and two that went straight from the machine to the garbage can. I would suggest three things,
(1) A pointed bit zero'd out precisly
(2) A flat table, resurface if you must,
(3) A high resolution photograph

Even after that not all pictures will look good, Try and find one that has lots of contrast.

Thats about it till I experiment some more.

[drodda]

Dan,

What material did you carve the picture of Diane in?

Thanks,

Dave

[burchbot]

Hi Dave
That is color mdf by Great lakes Mdf. I asked them for samples and they sent me 4 Pcs. !2"x12" I like it and want to get a 4'x8' x5/8 in black. My local lumber yard has been trying but so far no luck. That is why I don’t respond to a post earlier about Great Lakes mdf. It doesn’t matter how nice the stuff is, if you can’t get it. In all fairness to them it is new and I’m sure it will take awhile before it becomes available to everybody.
Dan
P. S. I did my own veneering. The veneer was select white maple.

[drodda]

Dan,

Thanks I have been thinking about trying that stuff. I guess I will wait till it is a little more accessable.

Dave