Pieces are coming out larger than Gcode

[cityguru]

I recently purchased a JCUT-1325B, man oh man am i going crazy. Support is a nightmare and the software they include NCSTUDIO is simple in design but the manual is not a big help.

Biggest issue we have right now is that everything we put into the machine comes out bigger than it is supposed to be.

By default the program puts in for Mobile Parameters .005, the company never bothered sending me the correct parameters when they sold me the machine, now that i am having problems little by little they are sending me pieces of info.

Anyway apparently for the JCUT 1325B the settings are
X: 0.00625, Y: 0.00625, Z:0.003125
And the maximum feedrate of Z axis , please change to 1000
The acceleration , change both of them at 400

Everything else i assume is default since again no other info i got from them.


So here is the situation, in this simple test (attached is the gcode), we simply cut a square hole which is 2 inches by 2 inches. We are using a 6mm bit. In the simulation in our CAM program it looks perfect. the from problem is that the size of the square when put into the machine is coming out approx to 3 inches.

originally when we put this in when the setting was .005 it was more like 3 and 5/8" after the .00625 it went down to 3"

I would figure perhaps this value is incorrect.

Of course in the Gcode everything is in millimeters, and you can check the G-Code attached, which is very small.

Maybe i am missing something here but i am pulling my hair out here.

If someone could take a look that would be great. can really use the help

[Butterknife]

Cityguru,

I own a JCUT6090A, but I did away with the controller and used WinCNC.

If you don't mind, I would like for you to make a measured move. What I mean is, lower your tool to the table, mark the location, lift, tell the machine to move in either X or Y direction for 500 mm (or as far as you can).

Next measure that line and post here what the length is. I think you should be able to do correct resolution = commanded divided by actual multiplied by current resolution.

So, say you commanded 500mm but it moved 400mm. Correct res = 500/400*0.005. Correct res=1.25*0.005. Correct res=0.00625.

Say you commanded 500mm but it moved 1000mm. Correct resolution= 500/1000*0.005. Correct res=0.5*0.005. Correct res=0.0025.

Remember to plug in the numbers you get. I can't promise this will work, but it's the way I do mine.

Good luck,

Butterknife

[wizzardworks]

There are two sets of perameters depending on which guideways were ordered. The X and Y can be either .003125 for the Nema 23 size steppers or .006250 for the NEMA 34 size steppers. Set them in the manufactory/perameters menu accessed by the password "ncstudio"
wizzardworks

[wizzardworks]

Originally Posted by wizzardworks There are two sets of perameters depending on which guideways were ordered. The X and Y can be either .003125 for the Nema 23 size steppers or .006250 for the NEMA 34 size steppers. Set them in the manufactory/perameters menu accessed by the password "ncstudio" wizzardworks

In the attached post I left something out. The first click on the toolbar is "windows" from that menu select perameters (third item from bottom or alternatively alt+F4) then
click the "manufactory button on the left. THen enter the password (NCstudio) and scroll down to the bottom.
As an example from calibrating my Z axis. I ran the spindle down close to the bottom limit and measured from the mount to the housing with a 12" dial caliper and got 6.187" then ran the spindle up 5 incremental moves of 10mm. This is the bottom one on the incremental moves. The measurement was then 8.158". The difference is 1.971" The actual distance should have been 50mmX.03937in/mm or 1.96850 The ratio 1.971/1.9685 is 1.00127 My Z axis perameter had been set at .004946. multiplying 1.00127X.004946 came out to .00475 which I entered in the z parameter box and clicked apply. Running the same check
showed the correct move to the accuracy of the dial caliper.
wizzardworks
.

[ProDrones]

So i have also some issues with calibration.
That thread helps me a lot because no manual with the machine :-(


So now i have made a simple milling piece and i have now 0.1mm to small parts.

ex:

CAD/CAM Hole Diameter: 12mm

CNC milled Diameter: 11.9mm


Stepper Settings on all axis: 0.003125


Can you tell me how i can correct that ? I think i must correct the value from x and y axis. Z is good.


Thx a lot

[wizzardworks]

Originally Posted by ProDrones So i have also some issues with calibration. That thread helps me a lot because no manual with the machine :-( So now i have made a simple milling piece and i have now 0.1mm to small parts. ex: CAD/CAM Hole Diameter: 12mm CNC milled Diameter: 11.9mm Stepper Settings on all axis: 0.003125 Can you tell me how i can correct that ? I think i must correct the value from x and y axis. Z is good. Thx a lot

Prodrones, Several possibilities. First I would mesure a longer length. I lay a piece of flat bar on the table up against the gantry upright and then use the bottom(10mm) incremental jog to move the gantry 100mm and measure that. For your example you appear to need a longer distance per motor step. 12/11.9 X .003125= .003151
You might measure your cutter diameter and make sure it is correct in the CAM input you are generating G-code with. Another factor is how much you input to leave for the roughing pass, and the tolerance input for how close to the target the tolerance is set. If you are useing a roughing pass did you use the same cutter for the finishing pass. There is also a scale factor in the CAM packages and also in NC studio. For measuring on setup the scale factors should be 1.000
I would measure the actual machine travel to set the machine perameters, then when that is correct sort out what the G-code is telling the machine to do. I would preffer that you check the machined part dimensions on a square block at least 3 inches square (or 80mm) cut out of something like MDF which gives a smmoth clean finish.
You can position a dial indicator on the flat surface on top of the spindle motor and raise or lower with a 10mm incremental jog to check that perameter.
wizzardworks