Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Bhohbein on April 04, 2015, 06:14:20 PM
-
Can someone run a bolt circle pattern on their machine and see if it works for them please
Im trying to drill a 4 hole pattern at 10 inches useing mill wizard. I drill 2 pieces and match them up to each other and the holes are in the same spot. But when i turn one 90 degres or flip it over and try and match them up again the holes are always off.
If someone could please try this and let me know how it works out, im pulling my hair out here trying to get this thing set up right
-
You may want to try the G16 method for bolt circles it will be as accurate as your machine is.
Just a thought, (;-) TP
-
Are the co-ordinates ok or is this a hard problem? Like backlash?
-
I dont know what the G16 method is ill do a serch on that in a min.
I dont know if the cordinates are ok Im useing mill wizard for the gcode .I dont know how to use any cad programs at the moment. Im trying to learn gsimple right now but Im an idiot haha
I dont think its a backlah issue. i keep checking for backlash with a dial indicator and its not there. ive tried setting backlash compesation at a couple thousandths and it just gets worse.
Ive set steps per unit a ton of time out to 11 inches with a dial caliper.
Ive checked for loose machine parts and everythings tight. Its a chinese machine but its pretty sturdy.
Ive even tried to do 2 2 bolt hole circles and change the degree on 2 of the holes 0.5 or 1 degree off and cant get it to line up.
-
I would make a test piece with co-ordinates that I calculated myself and see if the problem persists just to eliminate that possibility. Is the machine based on servos or steppers?
-
Im using stepper motors and a g540. i did a list of bolt holes wizard once but it was still off. I was doing a .406 hole with a .250 endmill so i tried a .250 hole and still has the same problem. I dont think im looseing steps or my steps are off i hit go to zero and it go back to the same place and the holes are always in the same place..
-
how far off are the holes ? Are they off in the radial mode. 4hole mode = 4 holes 90 deg apart radially.
Have you tired drilling a test hole instead of milling ??
When you say mill wizard is that the one that comes standard with Mach3 or one of the NFW ones ?
(;-) TP
-
Not the nsf wizards. Im using the mill wizard addon.. The holes are off about .040 to .070.. I did try just drilling a plain hole and still having the same problem. Ive even tried compansating with back lash and off setting the holes and still cant get them to line up when rotated or flipped over.. Im not saying i compansated correctly just saying I tried haha
Thanks for your help guys
-
Here is a simple G16 routine where MACH3 does all the math. Try it. It drills a center hole and a bolt circle of 5" radius 4 holes 90 deg apart.
G90
G0 X0.00 Y0.00
G0 X6.00 Y6.00 (move to center point of bolt circle)
G81 X6.00 Y6.00 Z-.250 R.250 F10 (drill the center point hole)
G16 (X will set a radius from the center point, Y sets the angle)
G81 X5.00 Y0 Z-.250 R.250 F10 ( Drill first drill point at 5.00"radius and at zero deg:3 oclock)
X5.000 Y90 ( rotate to 90 degress and drill hole)
X5.000 Y180 ( rotate to 180 deg)
X5.000 Y270 (rotate to 270 deg)
G80 (cancel cycle)
G15 ( cancel G16)
M30
%
-
Can I just copy and paste that code and run it.
-
YES you can. You do need to add a feedrate at the beginning say F10 or so. I did look at teh Wizards gcode for the same setup and it is correct. (;-) You may have a gantry that is out of line with the X axis.
(;-) TP
-
Ok guys Im really soory for being such an idiot but i copied it and tried to paste it in mach3 but I dont know where to do it haha. Really sorry im not a computer guy. Im not a machinist. Im just a mechanic I can figure most stuff out but Im just so fryed out on this stuff. Thanks again for all your help
-
Nevermind I found where to paste the code haha yay me.
-
Ok I pasted the code but had to change some of the inputs to fit the scrap material i have and screwed everything up but it did run and I noticed that instead of stopping at +5 on the dro it stopped at 4.9977. I know its only .003 away but could that be my problem.
-
Actually it was only .0003 off. That is due to step resolution. That is not your problem.
(;-) TP
-
OK a simpler test code. Set your center point to X0 Y0
g90
G0 X0 Y0
G81 X0 Y0 Z-.250 R.250 F10 (drill center point)
x2.5 y0
X0 Y2.5
X-2.5 Y0
X0 Y-2.5
This does 4 holes on a 5"bolt circle . Based at X0Y0 the math is easy to do. 2.5 " each direction from center. Change teh values to suit the size of the bolt circle.
(;-) TP
-
OK happy easter guys thanks for your help again. I inup the gcode and drilled the holes on 2 pieces and checked them they are off by .035 when one piece is fliped over if you get what im saying. so that would mean that my machine measurements are off correct
-
I dont really know if they are off on x or y but when i check the 2 pieces i check them the way they are cut. and everything lines up then just flipone over and line up the vertical holes and the horizontal holes are off. The hole on the right side is off in the downward direction and the left side is off in the upword direction. Almost like its turned 1 degree
-
It sounds like a mechanical issue.
Turn off backlash comp if you have it enabled and then do some tests to see if you have backlash and how much.
Also check to see each axis is moving the correct amount when you command a move.
Another thing to check is that your axis are perpendicular to each other.
Hood
-
I recalculated my steps per. i installed a screw in board on my table and measured against my spindle with a dial caliper to 11 in and was off .012 on y axis and .005 on x axis. and rechecked the bolt pattern. was off around .040
the backlash comp is off.
rechecked for backlash and is not showing backlash on x or y.. I know there should be haha . shook the machine by hand and there is nothing loose.
Used a dial indicator and commanded a move of .010 on x and y and it moves .010.
checked the axis for being perpendicular to each other it was off .120 but thats assuming that the table is square and i dought it. I just measured the table to the gantry arms. how should i measure that better.
-
Try cutting as big a rectangle or square as you can then measure the diagonals.
Hood
-
Ok i cut an 8 inch rectangle y length was 8.003 and x length was 8.005 measured from top left corner to bottom right corner 11.277 and from top right to bottom left corner 11.357
Is the problem with the table and how do I fix it.
-
I do not know how your machine is constructed so can't really say how to go about making it square but it would seem to be about 0.5 degrees out.
Hood
-
Its a signal ball screw in the middle with a rail on each side. i think i know what the problem is. I think the gantry is off and not square to the table. and i think i can adjust it. May take awhile but Ill let you know if it works
Thanks so much
-
Its fixed. The problem was that x was not 90 degrees from y. Stupid me should have thought of that. I was thinking that the gantry was square didnt even think thats the x axis could be a skew. I was able to slot the bolt holes on the gantry and adjust with a tsquare and is pretty accurate for right now. My plan is to make taller gantry arms later and the problem will be completely fixed.
thanks for all your help
-
Good you got it solved :)
I reckoned it was just under 0.5 degrees out from the previous dimensions you posted, doesn't sound much but as you saw it can make a huge difference.
Hood