Original X-Carve 1000m - Issues EVERYTIME I try to use it


I’m glad you are moving forward I knew Robert and Phil would get you moving in the right direction. I thought of another thing you should be looking at.

After you create a g-code file in Aspire and save it to your machine I would like you to open the file with notepad. Unless you are familiar with working with code it’s going to be gibberish but that’s ok your only looking at the first line and the last line. The very first line should say “T01” by itself, this is the software saying tool #1, it’s a command used in multi bit setups and is not applicable to use. I have seen and read about this Command causing problems in GRBL so please delete it. Then go look at the very last line and make sure it says M0(zero not the letter)2, so M02, that is the Command that says the job is finished but keep all of my zero settings please. If it says anything else please change it. Vectric fixed it in VCarve 8.5 so I don’t have do it anymore but I used to on every job.


I imported a file once Robert in Vcarve and used the trace bitmap Command and where smoothe curves were in the original I had so many jagged lines in the trace it looked like a hedgehog, took an hour to fix all the nodes.

This is GREAT! Seems perfectly conservative until I can do more experimentation! Do you ever use more than speed 1 on the Dewalt?

Thanks so much.

Ok, I’ll do that as well. Quick question. When I use Easel, when a job is done, it returns to 0. But, it turns off my spindle and vacuum. I am using this, which I found a while ago in this forum.

But when I create the g-code in Aspire, it doesn’t turn it off when the job is done and it returns to 0. I assume Easle adds some codes to the end of the g-code, but I am not sure.


I use the same relay box, go open a already saved g code file in notepad and look at the very last line, it should say “M02”, if it says anything else change it to M02 and try the file again.


I just looked at my X-Carve post-processor file for Aspire that I downloaded from Inventables. It has

begin FOOTER

“G0 [ZH]”
“G0 [XH] [YH]”

Doesn’t that add it to the end? And shouldn’t that stop the spindle?


It seems g-code generated with Easel has a M5 at the end, if I have it set to Automatic spindle. Should I use that instead?

Try adding - M05 S0 - to the end of your gcode, before the M30.

1 Like

I while back I was having all kinds of issues with having to reset my zeros after each Carve, along with some other erratic behavior. I did some research online and found that while M30 is a end job Command it’s not a great one and M02 is better. I can tell you that since I’ve started using it I’ve not had any problems with it. Also in Vcarve Pro 7.5 & 8 they automatically ended the file with M30, then when Vetric went to 8.5 they changed it to M02 automatically, that’s why I’ve brought it up. Phil is a computer guru maybe he can throw some input out there.

1 Like

I forget to add I use @CharleyThomas Triqureta block so M30 was really messing me up.

Curve fitting helps a great deal, especially if you’re using UGS. The motion planner on the XCarve hardware is basically an Arduino, so it’s amazing that it works as well as it does, but it has limits. The Arduino used by GRBL doesn’t have much memory, so it can’t look very far ahead while trying plan the motion. If you create paths with lots of very small line segments, the planner isn’t able to look far enough ahead to create a good motion plan, and gets stuck being really conservative. Fitting to curves or arcs cuts out nodes that don’t really contribute anything, giving you longer segments, and giving the planner a “longer view” of what’s coming, so it can do a better job.

If you use PC based control software, like Mach3, or use a newer controller board with more horsepower, like a TinyG or a SmoothieBoard, the motion planner is able to look further ahead and make better decisions, and will do a better job of handling files that aren’t set up ideally.

This is the kind of thing that often trips up newcomers, and what Phil says is right - The XCarve is a very good machine for what it costs, but that price point implies a number of concessions that had to happen to get it there. If you know what those limitations are and how to work within them, it’ll serve you well.

Read the forums voraciously, ask questions if you have trouble, and start small - Doing things like cutting test circles, crappy throw-away projects, and simple profile cuts is the best way to start, because you’re not investing a ton of time or emotion into it until you get the kinks worked out. Run projects in air first, then on test materials until those come out right, and then finally try doing them for real.

One final note, on feed rates - It’s more art than science. The rate you can push through something will vary according to your machine, belt tightness, motor size, current settings, acceleration rate, RPM setting, depth of cut, type of bit, number of flutes, type of material, humidity, and far more. Running conservative speeds is a good idea until you get a feel for how the thing sounds. I used to run every cut about 10% speed when starting it, then slowly dial it up to my ideal, or higher, as the project was cutting and I could hear it was going well. It takes trial and error (if you’re being aggressive, it takes a lot of error). Sometimes weird things happen, too - A piece of wood with a lot of moisture in it can swell as it’s being cut, exerting more force on the bit than if it was dry. If you run the RPM too high, the friction can build up excess heat and break the bit. Things like that can take some time to wrap your brain around, and they’re not always obvious. If you’re working with a new material, run small test cuts to get a feel for it first.

1 Like

If you use the Triquetra block and use Charleys new program make sure you have the M02 box checked when creating gcode.

You can use the $12 parameter to tune the arc (G2,G3) performance in grbl. Larger numbers give fewer line segments at the cost of not matching the curve exactly. The default value results in a tight fit to the curve using many line segments.

1 Like

I have been so frustrated with exactly this type of thing as well. I bought the top of the line Vectric software and so far i still have to use Easel to get thing thing to chew up my overpriced plastic clamps instead of carving the project. 1000 mm, DeWalt 611, autofocus has never worked, and this group just seems to say, “we love it so you’re wrong…”

The biggest issues I’m facing right now are the dust boot and the clamping / waste board.

I’ve bought two different dust boots now, neither of which fit. The Suckit shattered during installation and scrunched when trying to route a 2x4. The one I heavily milled to get it to fit comes loose every once in a while, leaving the router to shred its black material all over the workpiece until I stop the process.

Clamping over a waste board seems to require moving the 0,0 location of the workpiece out of the way of the clamps. This, in turn, means a couple of inch perimeter of waste on the workpiece board. Perhaps the dust boot is snagging on the clamps, which means I’m not wasting enough material on the project. And those metal things that came with the clamping kit must work somehow, but I’ve yet to find them useful in any way.

The Vectric software seems to be very nice, with even several formats of gcode output. But I don’t see anything that says which format Easel requires. And I keep seeing references to a universal gcode sender that would perhaps replace Easel, but haven’t found anything specific in where to find such, links, installation instructions, etc.

Meanwhile, I still have product to get out. And my Chinese laser, though smaller and quite a bit less capable than the theory of a US-made CNC router, is running circles around the X Carve.

Universal G-code Sender link

Scroll down the page to “stable builds”. Click on 1.0.9 to download it.

Unzip the file.

Download and install JAVA link

Double click on the .jar file located in the directory where you unzipped the files.

Phil, I have thoroughly enjoyed following your posts regarding the new board design. A rarity to find someone that knowledgeable on a topic, willing to spend time with newbies.

Might you be able to point to a link for this “ugs” I keep hearing about? I’ve been unable to locate it in my searches this far.

Thanks again

= Universal G-code Sender. See above post.

1 Like

I primarily use UGS unless I need the extra 4-5 inches In either direction I cannot do with my Vcarve Desktop version (limited to 25x25) anyways for using Vcarve I use the Shapeoko post processor but in version 8.5 they do have an Xcarve version as well. As for UGS I have always needed to go to GitHub (just google Universal Gcode sender and it will take you to the download) Lastly Phil I am wondering if your comment about the preview is what causes one of my issues. Basically I like the preview but have found that it usually messes the whole workflow between bit changes. I simply have become used to following a particular process. i.e. Place material and setup Spindle > Launch UGS and zero to my material. Close UGS and spin everything up (Vacuum and spindle. Basically my limit switches trip on the spin up steps) than start UGS again hitting zero before picking my Gcode file and off to the races. Finally after job finishes use UGS to home machine. Close UGS and change bit then start process again. Lots of work for that preview area. I might give it a go without it since really I only use it as a reference to how much more is left to cut.

Yeah it is most defiantly interference. I keep telling myself I will make a filter with a cap but yeah that just hasn’t happened yet. It would most likely not be an issue if I had used shielded cable but I went a cheaper route and used cat5e unshielded. But UGS does crash on me after a long job. Basically instead of moving the bit say .1 inch it moves it .0001 inch after a large job. Maybe I will break down and just create a filter one of these days :slight_smile: really a simple fix that or just get the correct shielded cable.