I have three problem now that I have the machine in and running that I seem not to be able to solve, at this time.
1. I can't seem to set and store fixture offsets? I want to save in the highest offset number the positions of my fixtureing plate, but can't seem to store anything but H1?
2. Z hights seem to be off? Tools are touched off correct and tramed right as they do come to a 1.0" safety hight just before doing and work. I check them with a guage block and there right. BUT when I program, with MasterCam, for a drill to drill down -1.3000 with a .4000" peck and .3000" retracted above the surface, it seems to go shallow? any idea's.
3. My machine has some built in perameter that won't let me peck drill anything less than .39366"? If I program in .3000" it faults out?
Any help would be grately helpful. Thank you, John
How shallow is the drilled hole? I think the parameters are setable on the parameters page. Which machine do you have? On the back up for the fixture offsets are you backing up the intire machine?. When I back mine up I can save it under what ever name I want as long as it has .bck at the end this works great with my grid plate (base plate) as well as tools you can number them and take them out ofthe machine and the next time you restore from that named .bck file it puts all the right tool info in
just install in the right pockets. Place the fixture in the right place (row and collom) and load program, now you are making parts in as little as 15 minutes I love it.
Verfer, thanks for the response. My system has been down for a while that's why it's taken this long to respond.
1. I would just like to save the "Align Axis piont" into H32 for my fixtureing that I'm planning on for multi-pallets. If I have that save as H32 X0 Y0, I can use that for ALL my production jobs and I know that that will always be that offset. I don't want to back-up my stuff, just save that fixture offset in something other than H1. Like if I have a vice on one side, and a small fixture on the other. Could save the vise as H1 and the fixture as H20 (???) or something to go between different programs.
2. Know as this peck drilling goes. On Friday I prog. a drill cyle thru MasterCam that has a peck at -.300. retract .300 out of hole, and peck at .300 inc. thereafter. WHAT A MESS. First peck was at -1.0000 and than at -1.2000 then every .3000 thereafter, but it also missed the bottom of the hole and drilled to deep by .1500.
Why is this? The drilling stuff has me really pissed as even my spot/center drill depth seem messed up, TOO DEEP? I compansated for this by changing the program to drill -.1000, but that wasn't hardly making a mark, so I switched the program to -.1400 and it went -.2???. Not a big deal right now, but it could have been costly. I like to spot/center drill deep enough to leave a countersink after the drill goes in.
I will be trying some helical interpilation tommorrow, we'll see how that goes?
At this time, I'm not worring about more than 21 tools, but I will be saving them at a later date?
As for the machine, it's a Arrow 500. I'm used to Fadal's, but I've heard good things about these controllers and machines. If all goes well and I feel comfy with this, might look for a larger machine in the spring.
Here is what you should check on the driiling cycles check the tip angle in the tools file and set to 180° and see if that puts a stop to the depth problem it is most likly adding the tip comp for the end of the drill and if you have already comped for the tip of the drill in the program then it will make the hole even deeper (I.E. the larger the dia of the drill the more depth it adds to make up for the angled part of the drill).
This was a new one to me too when I started working with the 2100 many years ago.
Now lets see about the set up and the of set for each set up.
The H# are relevant to the set up number as an fixture of set (I.E., "set up" being the pallet and the vise on the set up as an offset) or you could go the rought I use and set the set up to zeros and jest use the offsets as as the intire set up.
I use the offset in as set ups so as to allow me to run 3 double kurt vises with 6 "H numbers" that can be saved and called up at any time. Is this more like what you have in mine? If so transfer the numbers from set up to offsets for setup #1 and erase all the set ups / set to zero. Does this make sence or did I realy confuse you or mearly missed the point all together.
John, I will check that for the drilling and see if that helps. I think I get the jist of the offsets and will try that Monday. As for the time, it's 6:52 pm here. I'm by Buffalo, NY. Thanks, John
How much have uou looked around in the files on the machine? Do you have the offset groups short cutt (button) on the home page? or do you have to dig display/table menu/offset groups ? This puts all the offsets and multi set ups all in their relations on one screen much better than prowling around.
Oh another handy thing to know is the ability to place the table to the same spot at the end of the program no matter what setup/or offsets are present "G0 G98.1 X15.Y20" should bring your table to the center front for loading !!!! warning make sure you have plenty of tool clearance or no tool at all in the spindle or there will be no tool or fixture any more"
typ. Example of end of program that I like and it makes it much better for the Operator
(ME in most cases).
T0M6
G0 G98.1 X15 Y20
M30
I love thease machines ON THAT NOTE: be prepared for the Hard drive failer when you get a chance take the Hard drive out and have it gosted onto a new drive of the same type for safe keeping trust me we just went through this.
John, I will do some looking around. I know about the hard drive failers and I think I might have 2 ghost hard drives with this machine, but will double check.
What is this "G98.1" command? I don't recognise it. Also if you will, could you PM me your phone # and a good time to call. Thanks, John
The G98.1 is a machine position relitive to the front left corner (Home position) like I said its realy handy and dangerous as well.
Give me a call if you would like I should be here a while longer. If I dont answer it because I may not here it if I have a machine running. If you want I can call you if you
want to PM your #
John, been trying a bunch of things this week, some worked and some didn't. I did get the drill hole depth corrected. I have a .1 clearance in my Mastercam prog, therefore it changed the depth too a .1 shollow.
- No matter what I try, peck drill still starts at -1.0 inch? Doesn't matter if I prog. .3 or .5, they all drill to -1.0 before it will start to peck? DON'T LIKE THAT.
- Also, when I use the CONTOUR, "RAMP" cycle from Mastercam, it rotates areound the hole, just won't travel ANYWHERE in "Z" axis? I like to do 1.0" plus size hole with a drill, than hilical ramp down with a cutter to get final size, like say a large counterbore that .5 wider than the hole and -.5 down. I have used the manual program to helical ramp, but would like to know that Mastercam can program and run these.
Any thoughts? Maybe my post if NOT QUITE RIGHT? Thanks, John
The 2100 will do the helical moves just fine unfortantly it has to be called a little difrent than many others yo need the direction G2/G3 THE END PIONT X & Y & I & J & F and the Z depth and the K (pitch) . I always try to keep my lead "K" so as the number of turns come out right to my XYZ location I like full circles (I.E stop where I started in X and Y) less math that way, think of "k" as Z start to Z finish divided by number of turns.
OK, I got the piont .02 for K by 1.1( Z distance traveled )/55 (number of turns)
basicaly K(1.1/55) and this statment will work insted of "K.02"
as for the drill thing I would check the perameters on the machine some one may have changed them.
I hope this helps
here is part of my post set up in Esprite
EX_CIRCLE : IF(presdim(3)<> nextdim(3))
: IF(circledirection = 1) arctotal=(angleend - anglestart) ELSE arctotal=(anglestart - angleend) ENDIF
: kvalue=((presdim(3)-nextdim(3)) / (arctotal/360))
: N CIRCLEDIRECTION X* Y* Z* I* J* K__*(kvalue) F
: ELSE
: N CIRCLEDIRECTION* X* Y* I* J* F
: ENDIF
this unfortantly puts code for every 360° of rotation but it gets you there
John, a BIG thanks for all your help and understanding with this. I greatly appreciate this. I did learn that code/way to program the helical moves manually from the manual, YES I do go back and try to read the manual. I just don't know why it doesn't work with MasterCam V9.1.
I can do the helical part, and it's quite quick to do manually aswell, but if I was to do a large number of counterbore, like for a ejector plate with 60 counterbores, it doesn't become to feasible.
What I would like it a point by point way to check my parameters for the drilling, I haven't been able to find out how to set it on my own or in the manual.
I'm adding a piece of MasterCam code for you to look at for Helical movements. Can you look it over and see if there is anything that is missing. This code does run and will NOT fault out the machine, but there is NO Z AXIS movement, it just keeps going round and round, but never drops in Z. Here is the code:
This is a peek drilling cycle, well was programmed that way anyway.
Clearance 1.0"
Retract .1"
top of stock 0
depth -1.5"
Peek drill
1st peek .3"
subsequence peek .3"
peck clearance .3"
Hope this helps you see what I'm getting at. Thanks, John
There would have to be both an "K" and an "Z" onb each line of code for the helix I belive it would egnore the k if there is no Z movement. I think the fanuc will run the code you sent. Also K" will never be "-" it will always be a positive number as it is a lead angle.
and I did finaly look at the drill cycle "J2" is a varible distance and starts with what looks like 3* programed value + drill tip and works its way down to programed value.
I think what you are looking for will be "J12" this would run the programed "K value" all at the same increments all the way down.
Oh and in the "drill cycles" Z is incremental from where it starts at I think this is true on all the machines I have run. I would have thought that master cam would have added that in to the depth that is the "R value" pluss the depth.
Can you show copy and seend the master cam post proscessor file?
If its like Esprite I may be able to help with that helix.
LinkBack URL
About LinkBacks
Acramatic 2100 Problems 
