LinkBack URL
About LinkBacks
Anybody?
| | |
Im new to wire machines and know enough to get myself in trouble. My question is im doing a simple form tool and im getting dewell marks in all my inside corners. You can see the controll pause for about 3 seconds or so. Its only .0015 mark but i have to hold .0005 .
Any help would be great. Thanks
PS im programing at the control in g-codes.
Sub Program looks like this
g01x0y0
x-.085
x-.115y-.03
x-.2075y-.0381
x-.3y-.03r.005
x-.425y-.115
gog40x-.6
y.2
x.2
m99
Anybody?
is the machine an A325 or an AQ325? That will make a major difference. Also can you post the entire code with cutting conditions.
usually on the older machines you could have a little slop in the ballscrews or it is the machine leaving extra material in the corners. Try running the first skim pass twice and see if that helps. You can also reduces the comp between the first pass and the second. If you reduce it to much you will see overburn from the first to the second so dont over do it.
you can also reduce the speed of the first skim cut to help with the dig.
Im just wondering why the the machine actually stops for 3 seconds or so in the corners? You have any insight on this? Thanks for your input
it is cause when the machine is in a skim cut it hits more material than what should be in there. When it hits the extra material it bounces back and forth till it clears the material. Just like tool push in a mill. When the machine is in a skim cut there is no real energy in the pulse for any real material removal.
Ok that makes sense. Ok, bear with me im a 21 year cnc machinist trying to learn to run a wire machine.......lol. The machine we have will not run 3 or 4 passes so how would i run the first pass twice and then the finish pass? Can i loop it some way ?
Another question on reducing the speed are you refering to on time and off time? Like i said im green...lol. I know from playing around with on time i can change the speed ( or inches per minute ) .
Your machine is capable of multiple cuts. If you look in your database book you should see that most of the settings have a C number and H number for the first cut / second cut / third cut / fourth cut. What database do you have loaded up on your machine? Look at the COND file and that should tell you what version of the database that it is. When i mean slow the cut down you want the take the SF number and increase it by 1 or 2 points. On a Sodick wire the first pass is a variable feedrate. So if the SF is 0001 that is 30mm/min. The machine wont do 30mm/min on most cuts but that is the maximum allowed. So if you change the SF to 0003 you have set the speed limit to 15mm/min. Once the First digit of the SF changes the machine switches to a fixed feed rate. the reason the machine goes into a fixed feed rate is that the wire is no longer slowed by material in the way so it would go at the maximum and not allow the wire long enough to burn the material away. EDM does not care if it is conventional or climb cutting so keep that in mind when you are programming. Most people leave a small Tab stop and reverse the direction. All a tab is an area that you dont cut on the first pass. With that you are still holding onto the part and that allows you to make the skim passes that you want. SF on your machine should be as follows.
0 / 40mm/min
1 / 30
2 / 20
3 / 15
4 / 10
5 / 7.5
6 / 5
7 / 4
8 / 3
9 / 2
Posting Permissions
| | |
