What little hair I have left, is running for cover!! HAHA
When I set the tool at the beginning, I set both Zand X at zero. X just touching the material, same in Z. Then I back them both off .1 for clearance and reset both to zero.
Go to run the program, and the program thens backs the tool of an additional .320 and then starts to run the program. Again, air chips.
I will play with it again later today, and see where my mistake is at. At this point, I just would like to see something being cut. I have a piece of Delrin just begging to be machined!
Thanks again
Smitty
Smitty,
I noticed that you said that after you "touch off" the material, you back off the cutter .100 and then reset your Zeros.
Well....this may be why you cut so much air. Onecnc lathe will put .100 default clearance to your Zeros. ( you can change this, it's under the "Boundary selection" dialog box.
Check what value is in this clearance box, sounds like maybe you have a value of around .220. (your .100 plus .220 in dialog box = .320 clearance)
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
The boundry/countour section is set at zero. The BOUNDRY has me confused. What does it do, and how do I adjust it. I will try and post my drawing and NC file. If this comes through, I can render the drawing fine, and pull the G codes fine, but once on the machine all goes to heck.
Smitty, you will need to set your nc driver for incremental output if you want to touch off as you have been doing. If X0 is anywhere else but on the lathe centerline, you will be screwed in absolute mode.
Typically, we create start lines for our machines. There is a box in NCPost Output settings, Save options, which allows you to create and save some code for the start and end of your program. This is where we put stuff that we will always call:
G80 (safety cancel any drill in case of a program abort and restart)
G40 (cancel tool compensation in case of abort and restart)
G90 or G91 (sets your controller for an upcoming program written with absolute or incremental values).
G92 X___Z___
T___ M6(tool change command or tool offset call out)
There could be other codes for tool offset, but they should all be described in your controller manual.
Note: your controller will have a default mode upon startup, either incremental or absolute. Consult your manual. But regardless, it is imperative to define how the program is written within every program itself.
G90 or G91 mode affects your NC Post general settings for G02 /G03. You may have to change these settings depending on what you do. Check your controller documentation about it.
Typically, in incremental G91mode, all arc outputs will have to be incremental, but in absolute G90, they could be either absolute or incremental, depending on how your controller software is configured and designed.
Note: onecnc will not output a G91 or G90 code when you switch the NC Post from one mode to the other. YOU will have to make sure the proper code appears in your nc code after it is produced.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Smitty,
The boundary box is where you tell the program what you want to machine.
You can use a boundary box, (you have to draw this prior to opening the tool wizard), or most commonly you would use contour.
With contour, you select the "chain" or tool path that you want to machine, in the direction you want.
With boundary box, the program would machine every thing inside the box.
The clearance is set here. This adds clearance to your model, so the tool has room to rapid back to start the second, third, ect.... passes.
Normally you would "touch off" your part, in x and z, then set that as zero. Then add clearance in the boundary box.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Smitty,
HU brings up a good point.
If you are using anything but the centerline of the spindle for X zero, then there is going to be problems with absolute programing.
It is most common to use the spindle centerline as x Zero, as this is also most common the x zero for your drawings and parts.
Looking at your drawing that you posted, your part is drawn with the centerline at x zero. Then when you touch off the outside and add .100 to that, then set x zero there, you are (half the diameter of your stock + .100) to far above where you should be.
Example diameter of stock = .500
.250 + .100 =.325 (to far in X plus) = (lots of air and no cutting action!)
Last edited by wms; 08-03-2003 at 04:34 PM.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Ooohhh,
I think a light bulb just came on!!!
Be right back, time to go do some testing!
Smitty
Ok,
Pulled the tail stock back, and measured from the center line of the Spindle. Now that got me VERY close, but I still am unable to change the .3208 value, (thats how far the X pulls back before any maching takes place) without editing the G-code. I will edit the code and see what happens next!
Smitty
Originally posted by smitty
Ok,
Pulled the tail stock back, and measured from the center line of the Spindle. Now that got me VERY close, but I still am unable to change the .3208 value, (thats how far the X pulls back before any maching takes place) without editing the G-code. I will edit the code and see what happens next!
Smitty
Smitty,
How big is you stock and what is the largerst dimension of your part.
I hate to see you hand editing. We can figure out what is going on so you don't need to edit.
Please try and post your drawing file so we can all get on the same page.
.3208 may be ok if you have .500 stock and have .100 clearance.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Smitty,
What config file are you using?
Here's a shot of how you might need to set up your config file.
It's under Nc setup, top of your screen.
Looking at you code, it apears that you are using the Grooving funtion. Is that what you meant to use?
Last edited by wms; 08-03-2003 at 06:30 PM.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Here is my Config and a picture of the Part.
The balls are .300 wide, shaft is .170 wide. Total lengh is 2.361, ball to ball. I have a .05 fillet where the balls meet the horizontal lines
The extra shafts on the ends of the balls will be cut off later.
Helping the handicapped is over time!
Smitty
and the part
I use the "R" in absolute, that has been working so far, at least in the air it has
Smitty, if you want, try switching your NC post setting to incremental code before you generate the toolpath. I think you are still mixing together absolute code output from Onecnc with your incremental tool start position of X0 somewhere away from the lathe centerline.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Smitty,
Here's screen shot of your part and the code. Using a grooving tool, (.125 wide, .100 step over, .100 clearance).
As you can see it moves to .500 (diameter) for clearance. (.300 diameter of part plus .100 for clearance, (times two, .100 for each side,) equals .500 diameter.
Again the center line of part and spindle is x zero and the end of your part is z zero.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
WMS and HFD,
Thanks for all your help. I still have the problem. X comes out way to far.
I wonder if it is within my CNC controller program, but I doubt it.
It has to be something that I am missing, but I have spent way to much of my day, and all your time and effort for one day!
Monday is another day,
Thanks again,
Smitty
Smitty,
You are going to have to Zip up your program file and post it here so we can download it to our systems and see what is going on.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
I'll give that a try.
Just a shot in the dark here, but here goes
Smitty,
Look ok to me. I generated code with the config setup as I posted above and it looks good. Goes to the right clearance and the step overs are good. Compare the code in the screen shot to what you have. I you have something different then "tweek" your config to match what's shown. I don't know what you controler needs.
I can't see why this would come out to far in X, if you are using the spindle centerline as X zero.
Does your controler need Radius programing Instead of Diameter programing?
If it did then the tool would be coming out twice as far as it should be. Anything about this on their web site? Also when you were hand writing the programs did you use diameters or radius'?
And did you use incremantal programing or absolute?
Is there a way change the controler to use absolute?
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Posting Permissions
Reply with Quote