# First V-bit carving using Carveco



## difalkner (Jan 3, 2012)

Well, it's only been about 6 or 7 months since we bought Carveco and I finally watched enough tutorials to hack something out - yay!! I have been feeling guilty spending so much on software and not using it so I picked something that brings Fusion 360 to its knees - lots of text. I love F360, very powerful software. It does not handle text very well at all but it's the sweet spot for products like the Vectric line and Carveco.

Not wanting to use my pricey hardwoods I picked up a 12"x48" glued up board of Spruce/Pine/Fir (I think this is Pine) at Lowe's and figured I would start with that. This also represents only the second or third time I have had Pine in the shop in the last 5 years - it tears my allergies up like crazy!

So, on to the project; it's 9.5" x 12" x 3/4" thick, cut with a 5/8" diameter 60° bit, 100 ipm, 18k rpm, and cut with two passes. The first pass took most of the material and I did a follow up pass lowering Z by 0.005" to clean up any fuzz although there was far less than I would have thought for Pine. Cut time was about 12 minutes (per pass). I squared it off with the table saw rather than cut it out on the CNC.

The finish is Nitrocellulose sealer, sanded, one coat of gloss lacquer, sanded, Mohawk Van **** Brown glazing stain, sanded, final coat of semi-gloss lacquer. The finish took about 30-40 minutes including drying time.

Here's the finished plaque - 








Plunge router and keyhole bit for the hanging slot - 








I was surprised how cleanly the Pine engraved for this tiny logo, which is about 1.5" across, and cut with a 1/8" 60° bit - 








Using Carveco for the first time was kind of fun and a wholly different approach than using Fusion 360 but there's a lot I want to do with it, including some 3D work. Actually 2.5D, I guess, because the bottom will be flat. This isn't truly the first thing I have cut with Carveco but it's the first thing I can show. Last week I asked our pastor's teenage daughter to send me a photo of her and her new dog but didn't tell her why. So I took the photo and V-carved it and it came out really nice and she loved it. But since she's a minor I don't plan on posting any photos of that project.

Enjoy!
David


----------



## Pro4824 (Oct 17, 2015)

Outstanding David! Especially for pine.


----------



## Semipro (Mar 22, 2013)

Nicely done David


----------



## Herb Stoops (Aug 28, 2012)

Wow those different fonts are so clear and crisp. How do you get them black,spray paint the whole surface and then sand it off?
Herb


----------



## difalkner (Jan 3, 2012)

Herb Stoops said:


> Wow those different fonts are so clear and crisp. How do you get them black,spray paint the whole surface and then sand it off?
> Herb


Thanks, Herb! I was surprised they came out so crisp on Pine, too. Maple, no problem, but a soft wood? 

The darkness is a wiping glaze or glazing stain. I used a brush to put it on and wiped it off with a rag just as quickly as I applied it. Then I used compressed air to blow any excess out of the crevices and wiped it again, then sanded it with ROS and 400 grit. I gave it 10 minutes to dry and then sprayed the semi-gloss coat of Nitrocellulose lacquer. Works pretty good, actually.

David


----------



## RainMan 2.0 (May 6, 2014)

Nice work David


----------



## beltramidave (Jan 6, 2016)

Looks great David. Have been waiting to see something from you using Carveco. Once you get it figured out, if it is anything like Vectric's Aspire, you will be hooked.


----------



## difalkner (Jan 3, 2012)

beltramidave said:


> Looks great David. Have been waiting to see something from you using Carveco. Once you get it figured out, if it is anything like Vectric's Aspire, you will be hooked.


Thanks, Dave! It's supposed to be like Aspire and more, especially for what it costs, but I am just beginning to enjoy some of what it does. Like F360, I am certain it will do more than I will ever use. I hope I get hooked on it and get even _half_ as good as you and some other Vectric folks!

David


----------



## MEBCWD (Jan 14, 2012)

Looks real nice David. Pine is hard to V-carve and stain or paint because of bleeding but it looks like you got that problem overcome. 

I noticed you ran your keyhole slot horizontally not vertically and I'm glad you showed this good technique. 

When you cut the keyhole horizontally you can shift the project left or right to find where the project hangs correctly. If it was cut vertically and is slightly off the center of the project it is hard to get it to hang correctly.


----------



## difalkner (Jan 3, 2012)

Thanks, Mike! 

It never occurred to me to run the keyhole slot vertically but you are correct, if it's not dead center of the actual weight of the wood then it will hang crooked. I realized when I did the slot that I should have fed it the other direction because doing it the way I did it was trying to walk away from the board I used for a straight edge on the plunge router base. If I had fed it from the other direction it would have tried to feed toward the guide. I knew that from the last time I did this but just plain ol' forgot.

The way I got around it bleeding is that I shot two fairly decent coats of Nitrocellulose sanding sealer from two different angles each time to make certain I got enough in the carved letters. Then I shot a pretty decent coat of gloss the same way. Only then did I use the glazing stain and it is fairly thin so it only took a tiny amount. I wiped off the excess and then used compressed air to blow the remainder out of the letters. Then I did a final coat of semi-gloss and was pleased that nothing bled out of the letters.

David


----------



## BalloonEngineer (Mar 27, 2009)

Why didn’t you use Carveco for the keyhole slot as well? No worries about a plunge router running away. You already had it clamped down to carve the back side. 

Beautiful carve and great job on the finish. The more you use Carveco, the less you’ll like and use Fusion.


----------



## difalkner (Jan 3, 2012)

Thanks, Richard!

Didn't even consider that, don't even know how to set that up in Carveco. How do you tell it to enter and retract in the same spot and how do you set up the keyhole bit? Do you first make a pass with a 1/8" bit to clear the way and then follow up with the keyhole bit or do you cut it in one pass with the keyhole bit? What feed rate?

I don't think Carveco will ever replace F360, for me anyway. Maybe if I start doing more of this 'artsy' stuff with text and then I can see Carveco being used a lot, especially if I do some 2.5D carvings. But most of what I do just fits the F360 world and my way of thinking and designing.

David


----------



## Gaffboat (Mar 11, 2012)

V Carve Pro actually has a "gadget" that will make your keyhole toolpath. However without that, you need to draw a vector that doubles back on itself and returns to the original starting point, offset the end point by a few thousands of an inch. Set the tool path to plunge to the correct depth for you keyhole bit. When you run the tool path it will plunge at the start point, go to the other end, then return to the start point and retract from the surface. My crude drawing will give you an exaggerated idea of what I mean.


----------



## difalkner (Jan 3, 2012)

Makes sense - thanks, Oliver!

I was thinking it wouldn't be too difficult to just write the G-code in the MDI window in Mach4.

Using the top for Z zero and the entry point for XY zero I believe this would work without issue, assuming 75ipm is ok for the keyhole bit to plunge and cut. The red text in parenthesis is for those who don't 'speak' G-code but wouldn't be in the actual command. Also, I just wrote this and didn't test it on the CNC and I only speak basic G-code so if there's an error please let me know.

*G01 F75 Z-0.375* (lowers the bit at 75ipm to the depth of 0.375")
*X1.5* (moves in the X+ direction 1.5" at 75ipm)
*X0.0* (returns back to the entry point at 75ipm)
*Z0.75* (retracts the bit at 75ipm to 0.75" above the work piece)

David


----------



## beltramidave (Jan 6, 2016)

Very easy to hand code for keyhole hanger slot. Here is the code I use for a 1" horizontal keyhole slot, using a keyhole bit. Zero X & Y to CENTER of slot, zero Z to material surface. Bit will move 1/2" to the left, plunge down and move 1" to right and then back 1" to left and retract.

You can change values for a longer slot if you want or even make it vertical.

G20 G90 G64 P.01 G40
G54
G0 Z0.125
G17
M8
M3 S16000
G4 P4.00 S16000
G0 X-0.500 Y0.0
G0 Z0.2
G1 F10.0 Z-0.1875
G1 F40.0 X0.500
G1 F40.0 X-0.500
G53 G0 Z0
M5
M30


----------



## BalloonEngineer (Mar 27, 2009)

Dave, the Z plunge will depend on the specific bit you have, and I have the dwell for the spindle coming up to speed set in my controller program (Mach3 and Mach4 have it in the spindle setup). and I do not understand repeating the speed command, but that is basically the way I do it. Do you have M8 mapped to turn on your dust collection (instead of flood coolant)?


----------



## beltramidave (Jan 6, 2016)

Richard, I do have M8 set to turn on dust collection for my machine. I am using Linuxcnc as well, so somethings may be different. I am not a gcode expert by any means, just know enough to get by. I know that I do repeat some commands that may be modal, but sometimes it makes it easier for me to understand. I probably could have commented each line to help understand what is going on...

Yes, depth and feeds and speeds could all be different based on your machine and tooling. For any Vectric users, there is a keyhole 'gadget' too. I have not used it, though I do have it installed.


----------



## difalkner (Jan 3, 2012)

I just went out to try my simple 4-line code and it works just fine. I turn my spindle and dust collection on manually so I don't need/use those commands. I like simple so I was pleased to see that mine worked and I may give it a shot sometime soon.

David


----------



## J0seph (Dec 2, 2011)

VERY NICE JOB and GREAT SUBJECT!!!! I am looking at Carveco Maker as an entry level program to try. I have a 5'x8' CNC that I use in my cabinet shop with Mozaik software to cut all of our cabinets out. I just want to experiment with some lettering ideas. Do you think that the Carveco Maker would be a good place to start?


----------



## difalkner (Jan 3, 2012)

I think so, Joe. It's not very pricey and no commitment term, has plenty of features, and they're starting to get some pretty decent training videos out. Have you seen any of those? You'll find a lot of folks here with the Vectric line of products and I think either will do what you want without any problems. 

Vectric has a larger customer base but the buy in is greater at the onset. What is Carveco Maker, about $15 per month? That's not too bad to find out if you want to go that route. You can download V-carve to demo on your machine and see which you like better but for the monthly subscription of Maker you can actually use the product. 

David


----------



## honesttjohn (Feb 17, 2015)

We gotta get David to a machine that uses Vectric Vcarve or Aspire and then see what he says. lol


----------



## difalkner (Jan 3, 2012)

honesttjohn said:


> We gotta get David to a machine that uses Vectric Vcarve or Aspire and then see what he says. lol


Haha! I've always been a 'swimming against the current' sort of guy, what can I say!?! :grin:

David


----------



## BalloonEngineer (Mar 27, 2009)

Why would he downgrade from his Carveco? 

I do own VCarve Pro and Carveco - he's not missing anything. Just have to get him creating "artistic" or sign type carvings - Fusion 360 has really limited text capabilities. There's good money in signs! Here are some from one of my customers - and their prices. I just cut the wood - pass it on straight from the machine. She does the painting and finishing - best customer ever!


----------



## difalkner (Jan 3, 2012)

Those are some really creative signs, Richard - well done! Does she give you the designs or do y'all collaborate? 

Just for discussion's sake I do have to point out that I could do those in F360 probably quicker than I can in Carveco, at this point anyway. :wink:

David


----------



## Pro4824 (Oct 17, 2015)

I've read from multiple sources that some of the Artcam developers left Autodesk and started Vectric. Then Autodesk discontinued Artcam so the remaining developers bought the rights to it and rebranded it as Carveco. So..... if that's the case then it's pretty much all the same basic program. 
My only complaint is, if they all started with Autodesk then why didn't any of them incorporate Fusion 360's (Adaptive Clearing strategy) into Artcam, Aspire, or Carveco???? 😞


----------



## difalkner (Jan 3, 2012)

Richard has the history line down pat so maybe he'll post it here. 

On the CAM side, Carveco, Vectric, etc. pale in comparison to the options and capabilities of Fusion 360 in that regard. Carveco and Vectric may handle text, photo V-carving, and that sort of thing better but I wish Carveco had the CAM module from F360. Now THAT would be an awesome program! 

David


----------



## BalloonEngineer (Mar 27, 2009)

Pro4824 said:


> I've read from multiple sources that some of the Artcam developers left Autodesk and started Vectric. Then Autodesk discontinued Artcam so the remaining developers bought the rights to it and rebranded it as Carveco. So..... if that's the case then it's pretty much all the same basic program.
> My only complaint is, if they all started with Autodesk then why didn't any of them incorporate Fusion 360's (Adaptive Clearing strategy) into Artcam, Aspire, or Carveco???? 😞


Actually, they left Delcam to start Vectric around 2005. AutoDesk bought Delcam (who created ArtCAM sometime around 1995) around 2014, mostly for the Powermill line of software developed by Delcam for its, wait for it, HSM machining (up to 5 axis). So the HSM (High speed machining - adaptive toolpaths) technology in Fusion 360 came from the same company that produced artcam, which is the Carveco codebase. Carveco, in my opinion does have more efficient toolpaths than VCarve Pro/Aspire. The smart engraving had multiple roughing bit options before they were added to the Vectric products, and Vectric only uses it in vcarving, not pockets.


----------



## difalkner (Jan 3, 2012)

BalloonEngineer said:


> Why didn’t you use Carveco for the keyhole slot as well?





Gaffboat said:


> V Carve Pro actually has a "gadget" that will make your keyhole toolpath.





beltramidave said:


> Very easy to hand code for keyhole hanger slot.


This afternoon I cut another of these plaques and just for y'all I cut the keyhole slot on the CNC. :grin:

I used my simple 4 line G-code and it worked like a champ, far less effort than setting up the plunge router and everything that goes along with that.

So y'all have a new convert - from now on I will probably cut my keyhole slots on the CNC.

Thanks for urging me in that direction! :smile:









David


----------

