Page 1 of 3

Avoiding Machine Gotchya's

Posted: Tue Nov 20, 2007 3:20 pm
by TReischl
As I read the posts here, which are always informative, I keep seeing the one about "I don't know what is wrong, the machine is cutting too deep, not deep enough, seems to move over at weird times. . . ." etc, etc. As most of us know, this is RARELY caused by either VCarve (in fact, VCarve has NEVER caused this type of problem for me) or the machine controller software, MACH 3 et al.

What occurs to me is that a lot of us get caught up in the "speed" thing. We think we have to push our machines to the limit, or we are somehow not competitive. The only time that is true is if you are running your machine 24/7. In my case, my machine rarely runs a full 8 hour shift. It finally occured to me, so what if a part takes 2.3 minutes longer? I set my limits in Mach to something a lot more reasonable, and guess what? Never a problem, the machine just hums along, day after day. Since it does not goof up anymore, I now have confidence and can do other things while it is running. When it ran on the edge, I had to sit there watching it like a hawk.

This whole issue reminds me of an old saying:


Posted: Tue Nov 20, 2007 4:22 pm
by Bagzzz
I agree, I slow my cuts down alittle and the cnc does as you say "hum" along with no errors. I too used to watch the machine incase of screw ups.
I now know I can walk away and be more productive doing something else while the cnc routs alittle slower than full boar.

Posted: Tue Nov 20, 2007 9:16 pm
by WillyInAus
Yes I would agree as well, most of the problems that I have had are to do with me pushing the speed and also ramping the speed up whilst routing.

I am still playing though and thus learn from my and our experiences thats why I find forums invaluable.


Posted: Tue Nov 20, 2007 11:22 pm
by Greolt
This is a good point.

Very easy to get wrapped up in the "How fast is your machine?"

Acceleration is more important than rapid anyway.

Just to pick up on what Willy said.
When using FRO to adjust cutting speeds, Art, the Mach author, says it's advisable to adjust down rather than up.

So if you are in the habit of using FRO then stay at or below 100%


Posted: Tue Dec 18, 2007 5:18 am
by handcrafted
The turtle always wins... I bought my cnc (one time payment) instead of paying an employee every week. The way I see speed on the machine is that it can do a better job than I can at any speed. I set all my feed rates at 80 and have not had one issue since with my machine... and quess what?

I am getting lots done and great quality.

Posted: Tue Dec 18, 2007 8:47 pm
by TReischl
Gotchya #79. . . .

Double sided tape (A Blessing or a Creation of Satan?).

Yup, I use it, but I have learned. If you are not cutting deep, if you are cutting man made material, if you are very careful, it works.


Cut solid wood, you know, the real stuff, that used to have leaves, and you might run into some trouble. You do a relief type carving and you go about 3/8 inch deep, suddenly you notice something has moved! Sure enough, the wood cupped since stresses were relieved on one side only, and pulled that good ol' tape right up.

This is one to keep an eye on. Once again, as with most things in woodworking, there is no magic ONE WAY.

Posted: Tue Dec 18, 2007 10:51 pm
by Thkoutsidthebox
I've noticed this too with solid wood. It has to be really flat (Planed properly) before loading into the machine or there wont be enough area grab between the piece and the machine bed. I've found that wherever possible I'm sticking with the good old screws on the scrap edge, and keep the tape for times when thats impossible or for large pieces. On large pieces of solid wood (Especially hardwood) the weight tends to help prevent the piece moving. DOC and feed speed contribute significantly to the chances of that piece sliding ever so slightly and ruining a multi hour carving...this I also found out the hard way! :roll:

Posted: Wed Dec 19, 2007 4:05 pm
by TReischl
I forgot to mention, one of the things I do, if I must use tape, is to screw a few small pieces around the edges to help stop any shifting.

The one to really watch is when you start carving pretty deep on solid wood, it may have started out flat, but it does tend to cup and pull the tape. I try to use clamps for those jobs.

I just finished a sign, 20 X 36 that needed to be relief carved to .375. All went well cause I used clamps. When I loosened them down one side, the wood bowed up at least 1/8. This is ok for this sign, fortunately.

Posted: Tue Feb 05, 2008 5:45 pm
by TReischl
Gothcya #36

Constant Velocity, is it a good thing? Or better yet, what the HECK is it?

The short course on CV. With CV mode off: You command a position, the machine goes there. Example, cutting into a corner, you command
(you are starting at 0,0)


The machine actually goes to the positions.

With CV mode on: The machine does not actually go to X1Y0. Control software has something called the "in position tolerance zone". What this means is that when the position gets CLOSE to the commanded position, the next command line is executed. This results in a slightly rounded corner. Usually, this is very slight. However, if your machine is running at high speeds, it can be quite visible.

So, why not just turn off CV mode all the time? Because it will also make the machine "chatter" at higher feedrates. This becomes apparent when small moves at high speeds are programmed. (it can also happen no matter how CV is set due to control loop cylce time). Turning it off can also result in what appears to be overcuts on inside corners. Since the tool actually has to come to a stop at the commanded position, tool pressure is relieved and an overcut results.

What to do? I suggest running with constant velocity mode ON and taking a look at the angular settings for CV mode in your control software.

CV can cause a lot of head scratching, but once you understand it, your machine will run like a fine Swiss watch.

Posted: Tue Feb 05, 2008 6:00 pm
by TReischl
Gotchya #19: My machine is chattering! Grrrrrrrrrr.

Obviously, chattering can be caused by lots of things. One of the things you should check (especially if you have just started using a new machine) is how the CV mode is set. If that is fine, then you might want to try something else, like SLOWING DOWN.

Ok, so why slow down? Here is what might be happening:

All machine controls work pretty much the same. There is a program running that is in a continuous loop. In this loop, a bunch of things happen, like commanding the axis to move to a position, seeing if you pushed a button, reading a line of command information, updating the display. . .the list is actually quite huge. Doing all this takes time. The time it takes to do this is called the control loop cycle time.

Here is when chattering occurs due to the control loop cycle time: You command motion to a position and the motion takes less time than the loop cycle time.(Usually occurs with multiple short moves at high feedrates) Since the axis are not going anywhere until they are told to move again, the machine sits there, voila, chattering. Some controls use buffers to help avoid this, but those can be emptied out if the feedrate gets high enough. The obvious solution is to slow down. BUT. . . you may not have to slow down very much, just enough to stop the chatters. Try half the feedrate. If no chattering, try half the difference between the original and the new, until you are happy.

Really FAST machines, like sail cutters and lasers use parallel processing to achieve higher feedrates. One computer does nothing but watch and command the motion, the other one looks at all the other stuff. This reduces the actual cycle loop time. I am impressed with how short the Mach3 loop time is.

Re: Avoiding Machine Gotchya's

Posted: Wed Oct 27, 2010 10:27 pm
Speed should depend on the cutter used.... no point using a half inch spiral compression on a machine that cant go faster than 10 mtrs per min, you will get heat build up and a dull cutter very quick esp in ply or mdf. So I always use the ONSRUD feed rate (my bible) calulations based on material used and pass depth needed . The widest cutter you really can use on a machine that maxes at 10 mtrs per min (like mine) is 3/8 inch or 10mm. Larger stright and upcutters can be used as they generaly have slower feeds than compression.

1) Cutter
2) Vaccum
3) Speed of your machine
4) Size of parts being cut


Re: Avoiding Machine Gotchya's

Posted: Wed Dec 01, 2010 4:26 am
by dhellew2
Just a quick note about tape. Not all tape's are crated equal. By far the best tape I've found is from Shopsmith. Their tape is custom made by spectape and was created for lathe work. If the part is too fragile to pry it off the tape will loosen its grip with a few drops of MEK.


Re: Avoiding Machine Gotchya's

Posted: Sun Mar 06, 2011 6:16 am
by LouieAtienza
When I first started with my home-made CNC, I had issues being my Z travel was only 4", and I routinely had to cut 7/4 stock, leaving me less than .5" of safe Z. If I didn't pay attention to the initial Z or safe Z height, then sometimes the Z ran into the carriage going up and if I didn't watch what was going on, m piece was done! Now I make a habit of checking everything before starting the job, even just glancing at the G Code to make sure everything's cool.

I too was bitten by the spped bug. Theough I can rapid all axes over 400ipm, my table was shaking uncontrollably. I lowered the rapids to 165 on the X and Y, and 120 on the Z. Less craziness, got to help with the cut.

To lessen the chances of warpage, I try to use exclusively kild dried quartersawn stock, that I have aclimated in my at least a year. Even then, sometimes the wood is not fully dry. Sometimes for the sake of expediency some woods are dried too fast in the kiln, and they actuallly case-harden. Then when you cut, you get to the moist center! Sometimes because the way the wood is stored it's the complete opposite. The only way to know for sure is to have it in as controlled environment as possible, but of course this is not always practical. As a small guitar builder, I've accumulated wood over the years, and by the time I have a project to do, the wood has been in my possession for a few years. Of course, quartersawn may be out of the question if you want quilt or birdseye maple.

I've learned to use any mechanical means of clamping as possible. I never trust double stick tape. I use it sometimes when aligning a piece, but then I always use blocks, or cut a fixture out of scrap. I've made a few just for guitar bodies. Up until recently I was cutting necks manually, but now I'm making fixtures for them as well.

Re: Avoiding Machine Gotchya's

Posted: Sun Mar 06, 2011 7:51 am
by knighttoolworks
well speed does not always need to be fast but it may depending on how much you can charge for the job. Say you quote for 10 hours of work and you find it will take 11 or 12 at a slow speed you need to speed up a bit. So then trying to get the max speed without screwup really matters. I bid on this 40 sheet job of marine ply 3/4" and bid it for two passes at 180 ipm but my machine had to do it in three passes because the plywood was so dense. so that added several extra hours of cutting and it hurt in the pocket book. the faster you can cut the longer bits tend to last because your getting close to the right chipload. unless you have an industrial machine it is hard to get the chipload right for most bits.
I don't usually cut really fast most of the time. the fastest I cut is when I surface my table I do that at 480 ipm. and 3d when taking light loads and it is a larger job I crank the speed up.

Re: Avoiding Machine Gotchya's

Posted: Fri Oct 14, 2011 2:07 am
by Osric
I'm new to the cnc world (I just bought a used home-made machine) and need clarification on what you all are talking about.

The person I bought the machine from was a former engineer turned woodworker who built the machine himself and was quite proud of the how he had it set up for maximum speed. I got it home and, after noticing a lot of chatter on cut out pieces, decided one of the things I should probably do is slow things down. However, since I'm new to the cnc thing, I'm not really sure how to go about doing that.

Is speed controlled in the design program (Vcarve), or in the program that runs the cnc (in my case turbocnc...DOS version)? If it is in Vcarve, I would assume that it is in the section in the tools and that I would just need to adjust a feed rate and it would put some line of code in the export file, right? If it is in the turbocnc, what should I be looking for to slow down the feed rate? I haven't really adjusted anything that he had set-up (wanted to learn before I started screwing with the program), and don't really want to change something that will screw up what it is set up to do.

Thanks in advance for the help.