Relief Carving Machine Time

I have been playing around a bit with modeling relief carvings and I am wondering what machining time with the 1F people have been getting for this kind of work.

In the sample one I created, it wasn’t too complex, but it was a bit large (20"x12") and the 1/8" ball nose bit for the 3D contour (after the area clear), took over 6 days according to the 1F controller when I loaded the gcode.

I can’t tell if that is what it should actually take or if Carveco is just not doing a good enough job of managing the tool paths. It doesn’t seem to have rest machining (or at least I couldn’t find it), so would something with rest machining do a better job? I downloaded VCarve Pro, but the trial doesn’t allow me to use my own file to test it.

Anyone have some work they have done (perhaps a pic) and could share the time it took to machine it?

1 Like

For reference, I have a 24" x 12" 3D model (relief) with total carve times of a little over 3 hours broken down like this:

Clearing toolpath: 1/4" flat endmill taking 1:30:00 at 120 in/min
Finish toolpath: 1/4" ball nose endmill taking 1:40:00 at 150 in/min

For comparison, when I changed just the Finish toolpath to use a 1/8" ball nose endmill, Vectric was showing the time goes to over 4 hours. So, including the clearing toolpath, everything would probably take a full day of cutting time with 1/8" bits.

Hope this helps.


Going to have a lot to do with what you are setting for the cutting speed and step-over. Twice the step-over will half your time but leave a rougher surface. It can be worth it to sand that off rather than leave it to the ball nose bit to do the super fine cuts.

Carveco’s speeds are very conservative. Find out what your bit can actually do in the material that you are cutting. E.g if using the Jenny bits: Jenny 1/4 and 1/8 speeds and feeds from Cody's recommend chart - #6 by JDog

1 Like

This is very helpful information. How deep was your carving?

FWIW, I am not actually going to carve this image, I am just using it as an apples to apples comparison to see how Carveco, Fusion, and VCarve handle relief carving to decide what software I want to purchase. The 3D relief is 1.2" deep (so it is a pretty deep model). All of these setups were using the same bits, feeds and speeds specified by SpeTool.

  • SpeTool - W04005 Upcut Spiral Bit 1/4" CD x 1/4" SD x 1" CL x 2-1/2" OVL(SP-D1/4-1/4-U-FBA) Roughing
  • SpeTool; W01015 1/16" TD Tapered Ball Nose 1/4" SD x 1" CL x 2-1/2" OVL ZrN Coating(R1/32-D1/4-ZrN-FBA) Finishing

I realized this morning that I was using a 1/6" bit instead of a 1/8 as I said in my original post, so I went back in and re-did everything and made sure everything was the same between both programs. Fusion is being temperamental and just can’t handle the toolpaths required for relief carving of this size. It took 128GB of virtual memory before I ran out of disk space to calculate!! With that, I think Fusion is a no-go for 3D carving.

So, comparing VCarve Pro and Carveco using a 100mm/sec rapid feed rate and a scale factor of 2 the simulation time for each differs dramatically.

  • VCarve: 27 hours
  • Carveco: 58 hours

I have not calibrated my rapid feed rate and scale factor to my 1F (but I did up my max-jerk to 10,000).
When I load the Carveco file in, it shows my machining time to be:

  • Clearing Toolpath: 2h 50mins
  • Finishing Toolpath: 1 day, 10 hours, and 6mins

The toolpaths are now better on the 1F than reported in Carveco, which is interesting because that was not the case previously, in fact, it was significantly slower on the 1F. I did change the carving to raster instead of Z level, so perhaps that was the big difference(?). (Resetting the max-jerk back down to 1,000 didn’t make that much of a difference, either 1 day, 16 hours). Not sure now, how I ended up with 6 days. :thinking:

Here are the reports from Carveco and VCarve:

VCarve Pro


Carveco Maker+

Relief Dimensions:

Width: 20.00000 inches Height: 12.00000 inches
Min X: 0.00000 inches Min Y: 0.00000 inches
Min Z: -1.20166 inches Max Z: 0.00000 inches

Material Thickness = 1.2017 inches

Z Zero = Top of material

Machining Time: 58:05:55

Carve - W04005 Upcut Spiral Bit 1/4" CD x 1/4" SD x 1" CL x 2-1/2" OVL(SP-D1/4-1/4-U-FBA) Roughing

Tool: [1] 0.250 inches dia. slot drill
Feed Rate: 120.00000 inch/min
Plunge Rate: 40.00000 inch/min
Safe Z: 1.69461 inches
Spindle Speed: 12000 rpm
Stepover: 0.10000 inches
Tolerance: 0.00100 inches
Allowance: 0.00000 inches
Home Position: X:0.00000 Y:0.00000 Z:1.69462
Comments: Carve

Feed Rate Length: 17794.0 inches
Plunge Rate Length: 220 inches
Rapid Rate Length: 1037 inches
Machining Time: 05:16:21

Carve - W01015 1/16" TD Tapered Ball Nose 1/4" SD x 1" CL x 2-1/2" OVL ZrN Coating(R1/32-D1/4-ZrN-FBA) Finishing

Tool: [1] 5.4 degrees conical with 0.031 inches tip rad.
Feed Rate: 70.00000 inch/min
Plunge Rate: 23.00000 inch/min
Safe Z: 1.69461 inches
Spindle Speed: 12000 rpm
Stepover: 0.00250 inches
Tolerance: 0.00100 inches
Allowance: 0.00000 inches
Home Position: X:0.00000 Y:0.00000 Z:1.69462
Comments: Carve

Feed Rate Length: 110922.0 inches
Plunge Rate Length: 3 inches
Rapid Rate Length: 15 inches
Machining Time: 52:49:34

Machining time estimates based on a rapid feedrate
of 100.000 mm/sec and a time scaling factor of 2.00

I just got an email back from Vectric and they do not have a refund policy, nor will they load my file and provide me with the output, so I can’t test this without making a purchase. :pensive:

Would anyone with VCarve Pro be willing to load up my test file and send me the gcode files for each toolpath, or perhaps load the toolpaths in their Journeyman and let me know what the carve times are?

The .crv file is 14MB zipped.

Unfortunately that won’t work. VCarve will only cut a project created by the trial version if it was created on the same machine. :slightly_frowning_face:

I am not sure I understand this. From what they said, you can’t generate gcode files at all in the trial version unless the model is from an unmodified demo file.

Are you saying that, in addition to the above restriction, if you save a file with a model that was created in the trial version that a regular paid version won’t generate a gcode file either? I.e. it tracks where you created it and if it is from a trial version, you are also restricted?

Correct, if you try to use a separate machine.

If you use the same machine, then a file created in the trial can be opened in the paid version and then toolpathing created & saved.

So no one here can take your file, open it in our paid version and create toolpathing/GCode for you.

They do this so people won’t try to use the trial version as their production application and then just hand off the file to someone else to tool who then provides the GCode file back (which can’t be constrained to any machine or user due to the nature of GCode files). Otherwise I could offer a service to generate GCode for anyone using the trial versions.

I guess that makes sense, but for someone who is doing a deep dive evaluation, it makes it hard to do an aplles to apples comparison. I like that you have more time in their trial to really get to know how to work with the app itself, but to me, i would rather see how well it outputs.

What if I were to give you the stl file and the settings? It is a single object on a basic stock with two toolpaths. No editing, no crazy processing. Would you be willing to generate the two gcode files and send them to me (or tell me what the time you get on the 1F controller are)?

As it stands (with what i have been able to evaluate so far) it appears VCarve is a bit less stable than Carveco, and I am also having problems importing some DXF files. Most of the capabilities, however, seem to be on par with one another. There are a few niceties that VCarve provides (like better tool library management, laser module, etc.), but they are just niceties. The meat is in the output quality/machining code that is produced.

If i can just see how well of a job VCarve generates gcode, I think that would settle it. If it is anything like Fusion generated gcode, I think it will be an easy decision. Granted the paid version of F360 uses rapid moves, but the size of the gcode is multiple times larger than what Carveco writes out. Perhaps that translates to being a cleaner cut in reality, but I am unsure if the extra machine time is worth it.

Anyway, thanks for your help.

That’d work. You can upload it here or send it to me in a PM.

Not sure what’s up there. I’ve been using it for almost 10 years. I don’t think anyone puts Carveco on an equal footing with VCarve. There’s a reason VCarve is the big dog.

Awesome! Thank you for your assistance.

The 3D STL file is 244MB and zipped it is 127MB, so I am not sure if this board supports that file size. I actually downloaded it from CGTrader here is the link

I then just sized it to fit 20" x 12" with a depth of 1.2" (I think VCarve tries to load it in as 0.894 default) and did a roughing pass and a finishing pass using the toolpaths shown above. Pretty simple really. Hardest part is getting the file.

I am not sure what you mean about VCarve being the big dog. Is that for hobbyists or industry? Carveco was created in 2015 by the same group that created ArtCAM, which was the industrial big dog for relief carving. They kept all of the industrial requirements, but restarted the UI from scratch and that becomes apparent when comparing it to VCarve. VCarve (to me) feels very dialog box-y and antiquated compared to Carveco.

For example, when drawing a vector in Carveco, it puts handles on the vector that you can work with it immediately not just changing size, but also changing corner rounding. Sure, you can use the dialog box if you like but it is not required.

Here is a square drawn on the canvas and you can see I changed the shape and corner radii just by moving the handles around and never had to move my mouse outside the square (now an oval). I can do that edit now, or later after the vector is created.


In VCarve, I first have to place the vector using a dialog box, and if I want curved corners, I have to specify that type of object in advance, and that is also dialog box-y driven. Then in order to change the radius at some point later, I have to go into yet another mode (node edit). That workflow is much more complicated than in Carveco and why this is a tough decision for me.

Carveco in their mid-tier software provides some basic 3D modeling. With Vectric, you have to go to the top tier to do anything 3D related. Arguably, I would go to a dedicated 3D modeling tool to do heavy work, but occasional tweaks would be nice in VCarve.

In VCarve, they offer a laser module, which is very compelling. Although I do like LightBurn.

I am not here to start a debate on which is better, that comes down to personal preference…just what I see in my evaluation.

Found out the issue.

Apparently you have to know the format of the drawing inside the DXF file to know how to load it. VCarve isn’t smart enough to figure that out from the file itself.

I was picking Import Component from the Model menu and trying to load a DXF that apparently only had vectors in it rather than choosing Import Vectors option in the File menu. :face_with_raised_eyebrow:

~6 months ago I tried the demo of both and decided to go with Carveco Maker+. It did seem to be a more modern UI. Both products were very capable but I just felt better with Carveco Maker+. Unfortunately nobody has really done a good comparison of the two on a feature by feature basis, so I went with gut feeling.

Good to know. Now that you have used it for a while, what pros and cons do you have on it?

How do you like the quality of the output?
How has thier support been?
Did you go with the purchase or lease model?

The one concern I have had is that being a newer product, there is less of an existing user community and third party add-ons and such. Have you run into any issues with this aspect?

I’m running it on Windows 10 on Parallels Desktop on a Mac, that may affect what I’ve seen.

Because it is running under emulation the “Simulation” feature is slow compared to running directly on the same hardware. It’s not bad though, just takes a few minutes instead of <1. It uses openGL 4 which would normally hit a GPU directly but on my system it gets an emulated OpenGL 3.3 where parallels passes the requests to the Mac graphics system.

I’ve had a few crashes as well.

I’m not quite sure how to quantify the quality of the output. You’re doing a lot of work on that. Me, I seem to get what I told it to do so I’ve been happy.

I’ve had little contact with them for support. The one real time was through their forum when I was asking about the OpenGL thing. It warns me that my graphics are not optimal so I contacted them to ask about it. Took a couple back and forth to get a good answer that although I was on OpenGL 3.3 it would work fine.

It’s a subscription. Used the discount offered through Onefinity to buy the first year.

There’s lots of videos on their website and on YouTube. Their community does seem very quiet. Since it is based on ArtCAM there are some useful resources from that community as well.

I’ve never looked for third party add-ons. What would be needed?

I’ve recently bought an Ortur Laser master 3 and Lightroom. Lightroom is real nice and cheap. I don’t think I need my CNC software doing laser stuff. I have looked in to it with Carveco, it seems to have a laser toolpath but it is for 3D work. I.e. I think it must be designed for CO2 lasers for cutting Z level layers.

I’m just a hobby user, playing around with it for fun. I’ve done some V-carve lettering, v-carve inlays, 3D work, etc. I’ve posted one or two projects here before e.g. Post up them projects - #897 by Atroz

Thanks for your feedback. I am doing it for hobby as well. I guess the engineer in me tends to over analyze things. :smile:

I absolutely LOVE your cribbage board! That is soooo awesome!

I noticed the community forum was rather quiet for Carveco too. Not sure what to make of that.

My interest in add-ons is mainly around how robust the offering is and whether or not it can be extended. VCarve has a few gadgets (they call them) to do things like create spirals, making gears. The point is, it can be extended.

This is a very tough decision between the tools, I must say. I find this video VERY compelling for Carveco especially where it does fading using a brush (at 14:44) because I can see that being needed a lot when combining reliefs. I can’t see how that could be done easily in VCarve (perhaps Aspire does) using the dialog box method of adjusting reliefs.


1 Like

That is an Aspire feature. VCarve Pro uses existing STL files created in another program that you bring in as a component and allows some basic manipulation for heights, etc. but alteration of the 3D object is reserved to Aspire. You can also use Aspire to create the 3D object in the first place using 3D drawing tools.

This one?

You can also use the node editor to do the same thing. There are many different ways to do things in VCarve due to the maturity of the product. But it’s a personal fit thing in the end - the tool you’re comfortable with is the one you’ll be better off with.

I think you’ll find the resources available in terms of user community, forums, YouTube, extensions (both from Vectric and 3rd parties), etc. for Vectric are more robust than Carveco.

But like you said, it’s going to come down to a personal preference.

Yep! That is the file!

The test i was using that for was to not only see how each product machines, but how well they handle files that real artists create.

I am not that good at the “from scratch” artistry and this was decent size and free to test with. My stuff tends to be like 2nd grade stick men compared to some of the works I’ve seen out there. :rofl::rofl:

Appreciate all your insight into VCarve and willingness to give it a shot. You have definitely given me some things to think about during this eval.

Today’s project.

I needed a serving tray so I made one. Walnut, about 18.5 x 13 x 1" It’s a 3D carve. I drew the shape of the sidewall and then extruded it along a path to create it. Couldn’t have gotten that shape on a 2D program with just bits (unless you want to custom make a bit).

I just put a coat of oil on it, not dry yet and it will need another.

Took around 5 hours on the CNC.


Beautiful!! And the fact that you did this in one day (including milling) is inspiring. I am so slow in making decisions about my creations. I keep vascilating over design choices too much.

Where did you get your walnut from? It is so pricey here in Colorado. Pine is the only thing that seems reasonable here.