LinkBack URL
About LinkBacks
Make sure your Z value is a neg not pos. Some times is helps to reference the machine again when this happens. Last check your tool height in the tool table and that you're zeroing out with the correct tool number in Mach.
| | |
When I load g code into the 1100 computer, I reference the machine, set the Z zero with the tool touching the stock, then push the start button, it goes to the tool change position then after the tool change it comes down to within .550 and starts machining in the air. It used to go to the start or zero setting and start, now it starts .550 too high, this is the depth of the part in the cad program. If I click the z axis and put in .550 then it machines correctly and starts at the correct height.
I does the same thing on a .3125 part, after entering .3125 into the z axis it starts at the correct height, but if left at zero it will start .3125 too high.
The wizards work correctly (Mach)
I have looked thru Mach and sprut cam and dont see anything that would cause this.
Any help appreciated...
mike sr
Make sure your Z value is a neg not pos. Some times is helps to reference the machine again when this happens. Last check your tool height in the tool table and that you're zeroing out with the correct tool number in Mach.
It seems to always be off the thickness of the part after zeroing the z, I can put in the thickness of the part manually so that z reads the thickness not zero and it will start at the correct height, just doesnt make sense to me?Originally Posted by twocik
I tried a negative .550 and it started high as well. The tool height I need to check in Mach, but the write program works correctly.
thanks
mike sr
Hi Mike,
Do you have the TTS tool system? I remember in one of your previous posts that you had designated a ball end mill as tool #1. If you have the TTS tool system set with the granite block and height gauge you should have your touch tool as tool #1 in the Mach3 tool table with the height taken from the granite block and height gauge. After referencing the machine in Mach and then loading your program (G-code) Then when you set Z by choosing tool #1 in Mach3.
Check out the video on this Tormach web page...
http://www.tormach.com/videos_machine.html
The video is called "Tool Table Setup And Tool Change"
Sorry if this is not relevant to the equipment you have.
Gerry
Red hair and black leather, my favorite color scheme...
from Vincent Black Lightning 1952 by Richard Thompson
Where are you getting your code from ? cad/cam ?
It sounds to me like the Z zero in your g-code is the bottom of the part and you are setting your tool to the top of the part. That would explain why it is always off by the thickness of your part.
Make sure both the CAM and machine use the same Z zero.
Scott
www.sdmfabricating.com
I did get the Tormach tooling system with the machine, I set up the tool table today, at least the first ten of them, I still need more holders though, at the price I may make a few of them myself.
I havent had a chance to try this out yet.
I am still testing on wood so it isnt a real problem yet....
mike sr
I draw the parts in Alibre, then export to sprut cam and generate the code from sprut cam.
mike sr
I think Scott_M is likely correct.
When you have an issue like this your best bet its to study the code (I'm gaging from your question that your still learning g code so I'll explain)
Run the same program again doing everything the same. look at the Z value when the tool is cutting air and you think it should be cutting wood. If the Z is positive (Z.5) then your datum (Z zero) is set in your cam at the BOTTOM of your part. Nothing wrong with that. Just zero off the parallel (bottom of part) or (not good practice) touch the top and type ".5" into the Z DRO. Its bad practice because unless your dealing with stock EXACTLY that thickness you don't actually know where your zero point is... it may be .02 below your parallels.
If you zero the top, mach cuts air and the Z value in the code is "0" or negative then the problem is likely your tool offsets. A frequent mistake is to start the program, zero with tool shown in the "current tool" thinking its height has been called. it may not have been. I like to check my offset on the first tool by loading that tool, typing "1" into the current tool dro, then typing the current tool to make sure the height offset for that tool is loaded. then I jog to the work and see if the DRO makes sense. I get close to the work and the dro shows .02ish then I know the offsets are correct.
Another good practice is after you edge find, go to the MDI and type G0X0Y0 to move to your datum and check it against your cam datum (0,0,0). Just last night this saved me a scraped bracket. I trend to use the center of the stock as zero for X&Y on prototypes and onezytwozys. I use a Haimer and zero left side, find right side, click the X DRO, type "/2", hit enter. now the center of my part is X zero. great for ruining parts with out having to know the size of the stock while programing.
Last night I was cutting two identical brackets to hold the solenoid valve for my Kool-Mist unit. In cam I put the datum in the center of the bracket on top, then transformed the operations to the "right" by the width of the bracket. when I went to drill, counter bore, and tap the two parts I put them side by side in the vise, zero Y-, touch Y+, type "/2" into the Y DRO. then zero X+, touch X-, typed "/4" into the X DRO. That put my datum centered on the X and Y of the part on the left. I typed G0X0Y0 into the MDI and realized it was in the wrong place because I had actually zeroed the wrong axis. Checking it saved my part.
The absolute best thing you can do is learn G Code. Not just to be able to write it, but to read what your cam is putting out and catch mistakes in your cam set up or part programing. I review every tool change and the first 5-20 blocks of each one. then I load in mach and simulate run. LOOK closely at the DROs on that scene that show X,Y, & Z extremes. You can catch a lot from learning to read the g code. its easier than learning another language because there aren't that many words. print out the code, go online to the mach g code site and go word by word trying to figure out what you are telling mach to do. befor your know it your will read code faster than Rain Man counts toothpicks.
Sorry its so long but I hope it helps give food for thought.
Another tip along the same lines its to use the parallels as reference when your "top" doesn't exist yet.
Say your part is .4" tall. your cutting it from .5" bar stock. odds are your stock is NOT actually .500". An easy way to set this up is put your datum on top of your .4" part in your CAM. Make your first operation facing the part to Z0. Load your bar stock and ROUGHLY zero X&Y, them touch the top of the bar. Type ".05" (about half the total you need to remove) into the Z DRO. Run the first op. Now rewind the program. flip the part after de-burring. Touch the parallel and type "-.4" into the Z DRO and find your X&Y zero. Run program. Your part will be .4 tall regardless of stock actual size.
Best thing is if you have to re-zero for some reason you can zero on the top face and know its ACTUALLY 0 AND .4" from the bottom of the part and parallels. this helps to not have to know the actual stock size when programing CAM.
Thats what I am doing is putting the stock thickness back in after zeroing out the z.
I have learned some of the g code, I am new to this and my age is against me on the learning process, so its going to take awhile thats for sure.......
I will keep digging, I think its coming from sprut cam, I just need to find out what I entered that I shouldnt have ha!
mike sr
Hi mike, I would second Scott on this check the zero position on your cad cam software. I use rhino, MADcam and mach3. I move parts to the 0,0,0 coordinate in my modeling program and make sure it is below/at the z not above.
Flux
I think this is the problem, the drawing is dimensioned from the bottom of the part, now to figure out how to change it in Alibre......
Posting Permissions
| | |
