it's my first post here so - Hello everyone! I would like to ask you if you could help me with wrong size after cutting. I spent whole weekend trying to figure out what's going on there and I've decided to look into internet and ask here also. My problem is that machine is always 1mm missing both in X and Y direction when cutting. With the same adjustments on cnc controller (estlcam) and with the same miling bit (3mm diameter) I did several tests: - cnc program for 50*50mm square result was 49*49mm - cnc program for 100*100mm square result was 99*99 mm - cnc program for a plywood tray handle like in the picture below has a final dimensions 99mm (where should be 100), 24mm (where should be 25), 319 (where should be 320) and so on. uchwyt.jpg Finally I did the tray handle with good dimensions by cheating on machine by preparing .nc program with 4mm diameter bit (but real diameter ounted in the spindle was 3mm). But it's not a solution.... The software (both for .nc files preparation and for control of cnc and program execution) is ESTLCAM. Microstepping X/Y/Z are 1600/1600/800. Distance per revolution are 59,94mm/59,88mm/8mm. In jog mode when I put "X100" the machine is going exactly 100,00mm in straight line, when I put go "X1200" the result is 1200,00mm. In Y axis is the same, not matter if travel is small like 100mm or long like 1200mm, so everything seems to be allright with "distance per revolution" and microstepping. When the machine is executing some .NC program, altought it's written correctly, the results are always 1mm to small on X and Y. It's not up to resulution of the steps (distance per revolution), because in jog mode everything is fine I've just found few posts on some forums in the internet like "My OX CNC is always cut 1mm to much in xy", but unfortunately there is no any solution or just a comment how someone who had asked figured out finally what was going on.. I've taken note of that those question were up to big size OX (like 1000 or 1500mm size) and double belt solution....... so maybe this is a key: not really smooth movement because of "tight" assembly of Xtreme Solid Wheels on double belt + decceleration before corner when .nc program executing + 85% of intertia for X and Y motor set in ESTLCAM = reason of lost dimension(losts steps). When trying to measure travels in jog mode "X100" means go straight 100mm - so there is no corner, so different decceleration way and value.. Maybe. I don't know. It's just my idea right now. Have anybody heard about this problem and solution? Thanks in advance!! My machine is built with - 1500mm*1500mm v-slot profiles, - double belt (GT2-3m timming belt, pitch 3mm, 6mm width) & ACME rod 8mm pitch - Nema23 178.5oz/inch on each axis + 20 teeth pulleys - V-solid wheels - Arduino Uno R3 (original one, not a clone) + 4*TB6600 set to 1/8 - all wires with shielding: - from Arduino to TB6600 (step and dir) grounded on TB's GND pin - from nema23 to TB6600 (A+,A-,B+,B-) grounded on TB's GND
Did you tell ESTLCAM to use 3mm bit and did you tell ESTLCAM to cut outside the line for the whole piece and inside the line for the hole?
exactly. I did several test. Because I supossed that maybe there was some issue with "Part" (for outside shape) and "Hole" (for inside shape) option I also tried cut by engraving mode - I put the deep of engraving equal to board thickness. I used proper strategy of toolpath for inside and outside contour. Result was also bad - 1mm missing. After that I prepared g-code by myself in notepad and the result was the same - 1mm missing both X and Y....
It could be a good bet to contact Christian at: [email protected] at Estlcam, and see if he recognises this problem.
1) Has the machine ever cut accurately? 2) What did you do to tune the steps for the motor? Initially sounds like you need to calibrate the axis for steps, there could also be 1mm of backlash in the system as well.
Interesting, can you post one of your g-code files here as well? Also a screen shot of the tool setups. Might need to zip the code file. Thanks Gary
Measuring in the jog mode may be yielding correct dimensions but I wonder if loading the machine - i.e. milling a job, is unmasking backlash or something? I think I would try a milling job taking a very shallow cut and then measuring..
My advice would be to design a simile 2x2 square and cut it out of ply or mdf. Check dimensions. Really need to know if machine has ever worked correctly, or is this a new machine.
Forgive me, I hadn't enough time to give some feedback to you. I checked that lower belt (i'm running dual belt system) and it's not well attached to the v-rail's slot. When the carragies with pulleys were moving along the X or Y axis then there was something like wave in the bottom belt, don't know how to describe it better. Anyway bottom belt was not attached in every place and sometimes it was going up like a wave when carragie was moving, sometimes was flat and seemd to be attached, but wasnt. It was also the reason of the resistantce in movement of X and Y. I'm not still sure about if it is the reason of 1mm off in every cut, but seems to be. I agree with @Christian James that running .nc programs can unmask some problems and despite of good results in jog mode there are some problems with program execution. When any of carriages it's not able to move smoothly then during .nc programs execution the decceleration distance and percentage factor of inertia when turining on the corners have a lot in common with lack of milimeters in milling parts. Within today I will re-assembly belts and test. I will let you know final results. Regards
Hi szalonewrzeciono, make sure the lower belt is secured with the required 0.5mm of lift to get good interlocking of the belts. If the belt is just glued directly to the extrusion or taped with too thin of double sided tape then the belts will jump over each others teeth and cause issues. Cheers Gary
@Gary Caruso did you see it ? It's made with 0.13mm adhesive from 3M. When i was assemblying dual-belt for a first time I did use VHB acrylic foam tape from 3M which was 0.6mm thick. The result was that the surface of upper belt that has contact with pulleys was not so hidden in the v-slot, was a little bit to high. I suppouse that tape thickness may be depend on belt model or producer, maybe. Yesterday I removed lower belt, quickly and without any problem because the belt wasn't well attached to the v-slot. Something bad happend with VHB tape. I assembled once again the carragies but with single belt and seems to be much smoother and lighter to move on. Today I'm going to make some test. Seems that dual-belt was my problem, but still not so sure. I will let you know later. @CNCMD Previously machine's set-up was with dvr8825 stepstick and grbl shield. I was doing then only some engraving things and other stuff which didn't require accuracy. I did a precise milling only once with some problems also, but I finally did. I was considering this dificulty of not getting precise part like fault of lack of amperage for Nema23. So I can sum it up and say: no, machine never was too accurate
It seems odd that a belt fault can produce a consistent inaccuracy of 1mm all the time. I feel there may yet be another reason?
The fact that it's 1mm regardless of part dimensions suggest that it's either a mechanical or software problem, not an electronic problem. It could be backlash (though I suspect it's not, or rather a different form of overall machine lash), it could be gantry/z axis flex, it could be belt stretch, it could be any number of things- and potentially a combination of all of them. In software, it would be some kind of cutter comp, stock-to-leave, I-don't-know-what (since I don't use Estlcam) buried setting that's trimming 0.5mm off of an outside cut. An easy test would be to cut the exact same 50mm and 100mm squares at the exact same speeds and feeds but this time use half the DOC. What changes? If nothing, it's a software problem. If the value changes, it's a mechanical problem. What about if you make a square doughnut with a 50mm square inside a 100mm square, and tell the software you want the ring? Does the inner square then become 51mm? Then it's definitely software. If it's still 49mm, it's most likely mechanical (the machine being unable to pull the cutter through the material, in some form). Honestly, this seems like too heavy a machine to be using belt on anyway, the tension you're having to use to minimise stretch, skip and backlash will be damaging your motor bearings over time. Motors aren't designed to take massive, consistent sideloading. That's what bearing housings are for.
@Rob Taylor I've just finished milling of mentioned by you square doughnut. Outter square was 70x70mm. Inner was 20x20mm. .NC file prepared in ESTLCAM and next machinned with ESTLCAM Controller. The results was 69x69 and almost 21x21mm. I did it in PCV 5mm thickness, depth 2mm by one pass. Before I started milling I double checked v-wheels&eccentric nuts, also the tensions of belts. I also put a two long rullers and checked in JOG mode if machine is always getting desired point. X100 was exactly 100,00mm, X1300 was 1.300,00mm. Same for Y. Evrthing was allright. Next I started to do milling manualy: I was typing ccordinates one by one. diam. 3mm end mill. F1000, S10000 AZ-1 X73 Y73 X-73 Y-73 AZ-2 and so on, up to the AZ-5,1 The result was........... 69x69!!!!!!!!! I was suprised, moreover I had checked milling gauge of 3mm diam. end mill few days ago when problem had occured for a first time and width of the milled line was exactly 3,00 mm. I've checked it once again now by milling deep (about 2-3mm) line on my baseboard and another line on PCV and the width was 3,00mm, exactly like diameter of end mill. I did also some tests with DOC 0,5mm in PCV (so it was 10 pases for 5mm thick pcv). By .nc program or "manualy", with high speed like 2m/min and slowly 0,5m/min.. results were the same .....69x69. I do not understand anything now what's going on.... Tomorrow I will probably try with another CAM and controller...... but from the other side i'm not convinced that it could solve my problem when JOG mode is very accurate, milling kerf exactly fits the diameter of end mill. I wish that solution for this problem was so simple... Best regards
Can the spindle and the bit wobbling cause that deviation of dimension, when gauge exactly fits end mill diameter?
In VCarve's Tool Database, a 3mm endmill is set up so that it is 3mm diameter. I hope that you set up the 3mm endmill in ESTLCAM so that it is 3mm diameter or 1.5mm radius, not 4mm diameter or 2mm radius. If you already set up the 3mm endmill in ESTLCAM so that it is 3mm diameter or 1.5mm radius, try different software such as Autodesk Fusion 360 and GRBL Panel.
Please listen to me. I already said what the problem was. You need to adjust your steps. What value are you using for steps?
@CNCMD my values are: Nema23 (200steps/rev) + GT2-3M (3mm pitch) + 20teeth pulleys - Microstepping set on TB6600: 1/8 - Steps per revolution (in ESTLCAM controller) X/Y/Z: 1600 / 1600 / 800 - Distance per revolution (in ESTLCAM controller) X / Y / Z: 59,94 / 60,06 / 60,00 - values set by making different travels (100mm, 500mm, 1200mm) - and they match always in jog mode, for X10 or X1200 machine goes exactly where I want to. - Max feedrate: 9 000 mm/min - Acceleration distance: 10 mm (tried also different) - Intertia: 75% (already tried with values from 0 to 99%) But to be honest I do not understand what's wrong with my steps adjustment... @jeffmorris endmill 3mm is set up in Estlcam as 3mm diameter endmill. I tried also with 2mm diameter endmill which was set up as 2mm in Estlcam Tool List. The result was the same. 1mm off. There is no backlash on Z-axis. Spindle mouting is PLA printed with 100% infill, attached to V-slot Z axis profile with bolts. The spindle is attached to PLA mouting by pipe hose clamp hoops. It's robust
While I'm not sure I would call that a "robust" machine (), it's clearly more or less suitable for the task. The inner ring of your doughnut test being 21mm and not 19mm should definitively prove that it's software; if it was 19mm (or otherwise consistently low in relation to the direction of travel) then we'd be talking backlash and step calibration, but it's not. This time on the same job it went both too far and not far enough, demonstrating that it's clearly capable of putting the tool where it thinks the tool is supposed to be, even under load. Hence the point of the doughnut test. The most obvious option, as mentioned above, is that you have your CAM tool radius set up wrong- 2mm instead of 1.5mm. You say you've checked that though, and it's set up correctly. That only leaves odd things like cutter wear compensation being set insanely high, or maybe some kind of incomplete roughing-finishing pass sequence (where you have a roughing pass with 0.5mm stock-to-leave, but no finishing pass set up), or something along those lines. I'd assume the Estlcam guys would know more about the possibilities on that end of things, but that's where I would investigate, personally.
When I said robust I was thinking about spindle mouting made of PLA. There is no flexion on it. I would never say that cnc router made of aluminium profiles is a robust structure Just a while ago I've done some test with the square doughnut one again (70x70 outter, 20x20 inner), but I set up in Estlcam the diameter of the endmill with value of 3,5mm - so I've cheated machine a little bit. Real diameter of bit was 3,00 mm. Milled line on the baseboard had a width of 3,00mm. Next I've launched program. The results are: 70x70 and about 20,4 x 20,4.. something more than 20mm). I'm going crazy
Consider this. You're indicating that you made moves of 100mm, 500mm, 1200mm, and they always match. Not to burst your bubble but there is no way you are able to prove that measurement without a gauge to the level of accuracy that you desire. 1mm is small to see if your just lining up a v bit and running it along a ruler, which could have some variation as well. Here is my recommendation. Set the distance per revolution to 60. Cut a 2x2 square. Then adjust your distance by the variance.
OK, so look. I put 60,00 both for X and Y. I cut a 2x2 square, than measure and calculate new distance per revolution value. I put the new value and after programming controller I start milling. 2inch x 2inch square is exactly 2,00 inch x 2,00 inch. OK, but then I would like to cut 5x5" square (without any changes in the set up of controller like) and after milling I'm receiving 5,5 x 5,5. In jog mode when I say X58,2 (2") then the travelled distance is 58,20mm. When I put X100 then machine goes +/- 104 mm. Your solution it's not a key. I tried it few days ago because I was considering for a while my new set up with TB6600 like something different, unregular, where more important is distance per revolution value measurment during milling than in jog mode, but no. It's not working like this. Last two thing to check now: another controller like grbl panel (or something else? appreciate your recomendiations) and spidle (from electrical side). I'm going for a short vacation tomorrow so I will not have a chance to play with OX next days, but I promise to go back here and give you all the response what is the reason. Thank you Regards
Cut out a 100mm X 100mm square piece. Use a digital caliper to measure the piece. If the piece is 99mm X 99mm, divide 100 by 99 to get 1.010101. Multiply 60 by 1.010101 to get 60.60606. Enter 60.60606 into Distance per revolution in ESTLCAM software. Repeat for Y and Z axis. Repeat test and adjust Distance per revolution if necessary.
If it were steps/rev calibration, the offset would be proportional to the distance travelled, by definition. It would be travelling an extra/lesser number of steps for every mm it's programmed to move. It couldn't be 1mm under on 100mm, 70mm AND 50mm squares, not to mention 1mm over on a 20mm square. If it was off by 2mm, 1mm, and 0.4mm or something close to those, it would definitely be step calibration. As it is, there's no evidence to suggest that's the issue. It's consistently the same distance off no matter the distance travelled, and moreover is directly impacted by the CAM (because the direction of error changes depending on whether it's an inside or outside cut) which makes it a programming issue, not a control issue. I partially agree on the precision element; while it's generally accepted that you can eyeball down to basically half of your measuring tool's resolution- 0.5mm in this case, giving "distance travelled" with two decimal figures suggests a level of metrologic precision that isn't supported by experimental practice unless you're running glass scales and dial indicators. However, if he's moving along, say, a 4ft steel rule marked in mm graduations, it's perfectly possible that the machine is being measured to within a reasonable accuracy at the distances given. Can't be certain without pictures, of course, but it's easy enough to use an engraving tool as a pointer, and of course it's easy to measure a cut line because it doesn't move. I'm not sure I see any reason to doubt the veracity of the measurements. Measuring a cut-out piece to define the step calibration also only helps if the machine is cutting correctly in the first place. If the true steps are 59.96 but the machine is cutting undersize for another reason, changing the steps to 60.6 isn't going to fix the problem, only exacerbate it.
[QUOTE I've just finished milling of mentioned by you square doughnut. Outter square was 70x70mm. Inner was 20x20mm. .NC file prepared in ESTLCAM and next machinned with ESTLCAM Controller. The results was 69x69 and almost 21x21mm. I did it in PCV 5mm thickness, depth 2mm by one pass. ---snip.. Best regards[/QUOTE] Funnily enough, that's exactly what one would get if a 4mm cutter was used.
Reading through all the posts, There is one other thing I do not see mentioned, bit size being checked. Are you sure the bit itself is 3mm, and not a fraction bigger? I agree to look at all the options, but it sounds like the problem is so consistent at any size you try cutting. If it were the step/rev being incorrect, then the bigger the square you try to cut, the bigger the error I would expect to see. Try cutting any circles, both ID and OD? do you get the same error at different diameters?
which is odd because I calculate steps/mm as 26.6666 using GRBL settings calculator that is pretty fast. I got my OX up to 7500mm/min which is fine except for one small section of the X which has a tight spot and always caused lost steps at that speed. [/QUOTE]
