Juddering on backwards travel


So in the main my X-carve seems to be working well. The issue i’m having is when the router (Dwalt 611) is moving backwards in Y axis it sometimes starts to shake. Its like it skipping over the wood rather than cutting in. This then throws the whole thing out and it looses position. The problem is i can’t tell what is coursing the problem, the Y axis seems not to be moving and i don’t feel a vibration in it when it is juddering. I’ve added the M5 bolts between the Makerslides on the X axis however this hasn’t cured the problem. It only does it when moving backwards, forwards is find so is left to right.

Any ideas? Voltage to low? V-wheels to loose?

Make sure that the y axis maker slides are parallel along their whole travel, that was my issue at one point causing it to only bind up going forwards since my y rails were about 19" apart up front and 20" at the back. Also, try increasing the voltage too, always good to have a little more oomph, but I recommend getting copper vram heatsinks for the motor controllers if you turn it up much.

For clarification, is this when cutting, or when running free in air? If it’s when you are cutting, particularly in a slot, that makes sense because your bit is at least partially climb-cutting. For a normal mill, a climb cut is a good idea, it results in finer finishes. For the X-carve, it’s not a good thing due to the flexibility of the system. I’ve encountered the exact same problem, I’ve largely dealt with it with feedrate, router RPM changes, and wincing.

1 Like

Hi DanBrown, yes it is when cutting in a slot. When you say you’ve fixed with feedrate and router RPM, do you mean a slower feedrate and higher Rpm? or is this a situation where its better to move quickly but slow the router down?


I’ve had some luck with both methods, and also with taking a shallower, faster cut. Probably the “shallower-faster” method is the best… How deep are you cutting?

only 12.3mm in plywood. Shouldn’t be a problem i would of thought. I’m currently using a feedrate of 1400mm/min and a slower cut (speed 1 on the dewalt)

Hmm, that’s deeper than I would be going in a single pass, myself. I generally limit my passes to about 1D for a bit, which would make a quarter-inch bit about half of that depth. I’m usually running between 40 and 60 ipm at those depths, so about the same feedrate at my high-end as you are. Try pulling it back to about half that depth?

I generally make several fast, shallow passes, then a single full-depth finishing pass that cuts off ~1mm to clean up any “steps” from the multipass depth cut.

EDIT: When I get home this afternoon, I’ll pull out GWizard and get you some feed-and-speed data, if you don’t have it solved by then. :smile:

sorry no i meant total depth is 12.3mm i’m only doing 1.5mm per pass.

Dang, and it’s STILL shuddering? That is really odd! Perhaps push your depth down a bit, say 3.5mm or so, and switch over to a single-flute cutter if you have one? I’ve had good luck with single-flutes, they seem to chatter less for me. Probably because they’re closer to optimal chipload at router RPMs.

I don’t understand chipload. I need to do some reading up. I’ve only got 2 flute cutters at the moment.
I guess its the amount of material the bit cuts in 1 rotation V how much the flutes can clear in 1 rotation.

“Chipload” is basically the amount of material that each cutting edge takes off of the stock in each rotation. Every tool will have an optimal one. Too much, and you strain the cutter. Too little, and the edges of the tool rub against the stock, instead of slicing off clean little chips. The variables are number of flutes, RPM, and feed rate. The faster the feed for a given RPM, the more each tooth will take off. Same for slower RPMs, or less flutes.

Generally, the faster your cutter rotates, the faster you need to feed it to keep the chipload correct. Or, if you can’t feed it fast enough, you can decrease the number of cutting edges (flutes) to keep the chipload correct. Routers spin VERY quickly for the kind of cutters we are using, so they have to be fed FAST to keep the load correct. Of course, with a flexible frame like this, a proper feedrate tends to lead to frame deformation and chatter. It’s all a balancing act. :smile:

Ok, this is starting to make some sense to me now. I’ve found a excel spread sheet which someone has writting on the forum for 611 speeds V feedrate and chip loading.
I’m assuming birch ply counts as between a hardwood and soft ply, the sheet recommends a chip loading of 0.003-0.005 using a 1/8 bit. To get in that chip loading ball park i need to ramp the feedrate up to 2400mm/min (95inches/min roughly) and a router speed of 16400 rpm.

This is a lot faster than i’m running and i’m not sure my machine is that well setup yet. I think i’ll do some tests and cross my fingers

Here is the spreadsheet again, I have added some instructions to it.

CNC Speed Calculator for Dewalt.xlsx (18.2 KB)

Thanks, I’ve just made on addition as I’m a metric guy and put a extra a cell with a mm/min feedrate conversation to imperial.

I don’t want to speak to soon but so far… It’s not going too bad. Played with the power setting on the gsheild and upped the speeds. Keep the fingers crossed.

I just want to say, the Xcarve is a good bit of kit but the support of the forum is what makes it. Having a group of people to come and ask questions and learn from others experience is brilliant.

1 Like

I am glad to hear it is working. Good idea to add the metric column. Although you will quickly realize you do not need the spreadsheet, For 99% of work that can be done on the X-Carve the proper speed setting is 1 with some small bits needing a 2. The spreadsheet is just useful to help convince people that low setting are actually best on the Dewalt.

You are 100% correct about this forum. Without the advise and help of the smart and talented people that take the time to help others here I would never have got my machine working.

1 Like

Is this for real? So if I want to use a .250 2 flute I have to run it at speed 1 at 300 ipm? That seems to be an awful fast move speed. It isn’t that I’m calling you a liar, I just want to confirm how I’m reading this before I try it.

The X-Carve is not designed to move reliably at 300 ipm so no, I would even attempt that feedrate. The recommended chip load calculation is just that - a recommendation. You need to balance the recommendation with the mechanical limitations of the machine.

The most important thing to consider from the chip load calculation is that a low speed setting on the Dewalt is better than a higher setting.

In the end all that matters is how happy you are with the cut you get from the machine. If you want to crank the RPM up to 6 and set the feed rate at 30 ipm then go for it. If you like the results you get then keep using those settings. The chip load calculation is just another resource to help you find that “sweet spot” where you get good results.

In my experience I have found that keeping the RPM low on the Dewalt consistently produces better cuts so that is what I do. Keep in mind that the “low” setting for the Dewalt is a pretty fast RPM for most dedicated spindles.

1 Like