First 'seriuos' attempt at wood carving

[Mountaincraft]

Worked on modifying one of Vectric's free project for a good part of yesterday, trying to resolve some issues in replacing their carved artwork in the middle with a 3D carving, and was finally successful..

So last nite, I found an old piece of pine out in the shop to try this out on.. It had been edge glued and was slightly cupped, so I screwed it down and then took 50 thousands off to surface the part of it where I was going to route the file...

Pine probably isn't the best material as it created a lot of 'hair'.. I ran the CNC file a second time over the relevant parts to clean it up some which helped...

One problem I had was that the first pocketing of the large open areas of the dish where the cross is, had a 'lot' of plunge marks.. I've sanded most of them out, but you can still see someof the hard to get to ones..

Is this 'typical'.. or is it a matter of using slower plunges (currently at 15-30 IPM) or a different bit (1/4" single flute compression spiral)..

Also, on some of the more intricate parts like the tips of the little detail parts coming out of the flowers, the pieces blew off here and there, also in one corner of the V Carve area.. I'm hoping this has more to do with the material being cut than it does the process, and when I do it in hardwood, these problems will disappear..

I'd like to get more detail and cleaner cut on the 3D elements.. but this also might be in part due to the material being cut.. I don't know.. I used a 3/32" ball end to do the finish pass.. but I might slow it down a little (currently at 200 IPM) and increase the step over (default)...

Anyways, any and all advise appreciated, like how to clean 'this one' up some more (can't find my dremel set.. will keep looking), and how to avoid these problems in the first place...

Thanks,
Mark

Here's a pic of it (the defects are more noticeable in person)

[CNC Lurker]

You might try slowing it down a lot, like around 60-70 ipm and see if that helps. I did that on some of the 3/4" pine craft board that Lowes sells and it came out pretty good.

As for getting rid of fuzzies, sanding sponges will get rid of most of it. They're cheap at Harbor Freight, and you might want to try both fine and medium grade sponges. I just rub the face back and forth with them. They also make some that have a bevel that might help get in grooves, but I haven't used them.

Pack of 10 Fine Grade Aluminum Oxide Sanding Sponges LINK

[Phife]

3d work is really a pain to do in wood, you'll find you will pretty much always get chips, fuzz, chunk outs and tear out with wood when 3d machining. Its better in some woods, but you will find its pretty much going to do it on all woods.

For your plunge cuts set up a ramping plunge, that should help with some plunging marks, also if possible a lead in helps a lot too.

Your issue with Z plunges is probably cause by a misalignment in your Z, its probably not perfectly perpendicular to your table, did you check your routers tram by putting in a dial indicator into your collet and turning it by hand on a surfaced board?

I used to do a ton of 3D work in wood, and now I only do it in 20-30# HDU.

*Edit* I usually run my 1/8" ball nose at around 200IPM, and 120IPM for my 1/4" Downcut. I prefer down cuts to up cuts, never tried a compression bit as they are more for full depth profiling.

[DonFrambach]

I'm certainly no expert but I have had success by doing things quite a bit differently.

I use:

1) hard, close grain woods work very well. Hard maple for example.
2) small bits, high rpm, slow feeds work well.
3) rough with a small bit and use shallow passes.
4) finish cut with a small bit with 4-7% stepover.

Here's an example using african mahogeny (I made another, better one with hard maple) 1/8" roughing and finishing bits, 10k rpm (because that was as fast as the spindle I had then would go), 20ipm feeds (I would have gone faster if my spindle rpm's were greater). The edge and the rings were "carved". The lettering was done with a 60 degree v bit.

[CNC Lurker]

Originally Posted by DonFrambach I'm certainly no expert but I have had success by doing things quite a bit differently. I use: 1) hard, close grain woods work very well. Hard maple for example. 2) small bits, high rpm, slow feeds work well. 3) rough with a small bit and use shallow passes. 4) finish cut with a small bit with 4-7% stepover. Here's an example using african mahogeny (I made another, better one with hard maple) 1/8" roughing and finishing bits, 10k rpm (because that was as fast as the spindle I had then would go), 20ipm feeds (I would have gone faster if my spindle rpm's were greater). The edge and the rings were "carved". The lettering was done with a 60 degree v bit.

Beautiful work Don!

[louieatienza]

Originally Posted by Mountaincraft Worked on modifying one of Vectric's free project for a good part of yesterday, trying to resolve some issues in replacing their carved artwork in the middle with a 3D carving, and was finally successful.. So last nite, I found an old piece of pine out in the shop to try this out on.. It had been edge glued and was slightly cupped, so I screwed it down and then took 50 thousands off to surface the part of it where I was going to route the file... Pine probably isn't the best material as it created a lot of 'hair'.. I ran the CNC file a second time over the relevant parts to clean it up some which helped... One problem I had was that the first pocketing of the large open areas of the dish where the cross is, had a 'lot' of plunge marks.. I've sanded most of them out, but you can still see someof the hard to get to ones.. Is this 'typical'.. or is it a matter of using slower plunges (currently at 15-30 IPM) or a different bit (1/4" single flute compression spiral).. Also, on some of the more intricate parts like the tips of the little detail parts coming out of the flowers, the pieces blew off here and there, also in one corner of the V Carve area.. I'm hoping this has more to do with the material being cut than it does the process, and when I do it in hardwood, these problems will disappear.. I'd like to get more detail and cleaner cut on the 3D elements.. but this also might be in part due to the material being cut.. I don't know.. I used a 3/32" ball end to do the finish pass.. but I might slow it down a little (currently at 200 IPM) and increase the step over (default)... Anyways, any and all advise appreciated, like how to clean 'this one' up some more (can't find my dremel set.. will keep looking), and how to avoid these problems in the first place... Thanks, Mark Here's a pic of it (the defects are more noticeable in person)

That looks pretty good for a first attempt. I think cleaning the floor up is more a matter of sweat equity. Since the grain lines in pine are harder in density, they'll wear less than in between if you use a soft abrasive pad.

Also, because the board was "cupped" and you just surfaced one side, there was probably an air gap toward the center on the side against your table. That will vibrate and flex when the tool plunges down and cuts. You'd either have to surface boh sides, or support the back with shims or such (maybe even hot melt glue.)


Some of the best woods to use would either be short grain, closed pore but relatively lightweight woods like basswood or alder or even poplar. Also if you have caviar tastes, rosewoods generally carve well...

Also check your z and tip of your v-bit, even check it's true angle versus it's marked angle...

[br1]

Not bad for a first try! Keep at it, it's a good start. Did your vector art have clean smooth arcs or were they line segments? Perhaps take a clean up pass say .005 deeper

[ger21]

Where's the pic. I didn't have time to look at it earlier, and now it's not there??

[Mountaincraft]

Originally Posted by ger21 Where's the pic. I didn't have time to look at it earlier, and now it's not there??

It is for me... That's odd...

Here's a direct link to it... Paradise Box Lid

[robe_uk]

Yeah I had a problem seeing it earlier but can see it now, maybe a problem with your hosting site.
Good job for a first attempt.

Keep at it

[ger21]

OK, now I see a message "connecting to " your site, and it finally loaded after a few refreshes.

harder woods cut with much less to no fuzz.

What I do is rough with a 1/8" ballnose. 1/8" deep and .11 stepover, across the grain at about 175ipm.

I finish with the grain, with a 1/16" ballnose and .005" stepover at about 150pim.

I've got some 1/32" ballnose, but haven't used them yet.

[Phife]

Also if your cam program has the option, I like using the offset spiral method of machining vs raster. Offset tends to leave less scalloping on inside edges, I use Artcam for my 3D work and it even has 3D offset which really helps clean up the 3D work at the cost of machining time.