603,853 active members*
5,159 visitors online*
Register for free
Login
Page 1 of 3 123
Results 1 to 20 of 41
  1. #1
    Join Date
    Sep 2005
    Posts
    84

    Cool Acramatic 2100 Problems

    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 :cheers:

  2. #2
    Join Date
    Aug 2005
    Posts
    197
    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.

  3. #3
    Join Date
    Sep 2005
    Posts
    84
    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.

    Thanks, John :rainfro:

  4. #4
    Join Date
    Aug 2005
    Posts
    197
    Ok,

    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.


    And just what time is it there 5:30 PM here? LOL

    John

  5. #5
    Join Date
    Sep 2005
    Posts
    84
    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

  6. #6
    Join Date
    Aug 2005
    Posts
    197
    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.

    good luck and keep me posted

    John

  7. #7
    Join Date
    Sep 2005
    Posts
    84
    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

  8. #8
    Join Date
    Aug 2005
    Posts
    197
    the pm was sent.

    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

  9. #9
    Join Date
    Sep 2005
    Posts
    84
    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

  10. #10
    Join Date
    Aug 2005
    Posts
    197
    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 example :
    :T1M6
    S1000 M13
    G0 X1 Y1 Z1
    Z.1
    G3 X1 Y1 I0 J0 Z-1. K.02 F25.0
    G3 X1Y1 I0 J0
    G1 X0 Y0
    G0 Z.1
    M30

    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

    you most likly new all the above

    Let me know what you find out

    John

  11. #11
    Join Date
    Sep 2005
    Posts
    84
    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:

    :
    (MSG, TEST )
    (MSG, T6 1.0" Helimill )
    N10 T6 M6
    N15 G0 G90 H1 X-7.8028 Y9.4063 S1300 M3
    N20 Z1.
    N25 Z.1
    N30 G1 Z.03 F15.
    N35 G3 X-8.3848 K-.0175 I-8.0938 J9.4063
    N40 X-7.8028 K-.0175 I-8.0938 J9.4063
    N45 X-8.3848 K-.0175 I-8.0938 J9.4063
    N50 X-7.8028 K-.0175 I-8.0938 J9.4063
    N55 X-8.3848 K-.0175 I-8.0938 J9.4063
    N60 X-7.8028 K-.0175 I-8.0938 J9.4063
    N65 X-8.3848 K-.0175 I-8.0938 J9.4063
    N70 X-7.8028 K-.0175 I-8.0938 J9.4063
    N75 X-8.3848 K-.0175 I-8.0938 J9.4063
    N80 X-7.8028 K-.0175 I-8.0938 J9.4063
    N85 X-8.3848 K-.0175 I-8.0938 J9.4063
    N90 X-7.8028 K-.0175 I-8.0938 J9.4063
    N95 X-8.3559 Y9.28 K-.02 I-8.0938 J9.4063
    N100 X-7.8028 Y9.4063 I-8.0938 J9.4063
    N105 X-8.3559 Y9.28 I-8.0938 J9.4063
    N110 G0 Z1.
    N115 X8.3848 Y-9.4063
    N120 Z.1
    N125 G1 Z.03
    N130 G3 X7.8028 K-.0175 I8.0938 J-9.4063
    N135 X8.3848 K-.0175 I8.0938 J-9.4063
    N140 X7.8028 K-.0175 I8.0938 J-9.4063
    N145 X8.3848 K-.0175 I8.0938 J-9.4063
    N150 X7.8028 K-.0175 I8.0938 J-9.4063
    N155 X8.3848 K-.0175 I8.0938 J-9.4063
    N160 X7.8028 K-.0175 I8.0938 J-9.4063
    N165 X8.3848 K-.0175 I8.0938 J-9.4063
    N170 X7.8028 K-.0175 I8.0938 J-9.4063
    N175 X8.3848 K-.0175 I8.0938 J-9.4063
    N180 X7.8028 K-.0175 I8.0938 J-9.4063
    N185 X8.3848 K-.0175 I8.0938 J-9.4063
    N190 X7.8316 Y-9.5325 K-.02 I8.0938 J-9.4063
    N195 X8.3848 Y-9.4063 I8.0938 J-9.4063
    N200 X7.8316 Y-9.5325 I8.0938 J-9.4063
    N205 G0 Z1.
    N210 M9
    N215 M2

    I know it's a little long, but it give you the idea at what I'm looking at.
    Here's the breakdown on the code:

    Clearance 1.0"
    Retract .25"
    Feedplane .1"
    Top of stock .03"
    Depth of -.200"

    Ramp parameters are, .035" per depth, or .035 depth per rotation.

    The other parameters like speed and feeds you can gather but that not important.

    I think my machine get messed up with the "FEEDPLANE" in MasterCam. If I have a .1 feedplane, than the hole depth is .100" shallow. Like this:

    N90 T2 M6
    N95 G0 G90 H1 X-8.0938 Y8.1113 S820 M3
    N100 Z1. M8
    N105 G83 Z-1.5 R.1 W1. K.3 J2 F7.
    N110 Y-8.1113 W1.
    N115 X8.0938 W1.
    N120 Y8.1113 W1.
    N125 G80
    M01

    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 :cheers:

  12. #12
    Join Date
    Aug 2005
    Posts
    197
    Ok,

    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.

    John

  13. #13
    Join Date
    Sep 2005
    Posts
    84
    John PM me a email address and I will send my post to you. Thanks for the info above, will look into the helical stuff Monday. Thanks, John

  14. #14
    Join Date
    Aug 2005
    Posts
    197
    John,

    Any luck with the changes?

    John

  15. #15
    Join Date
    Sep 2005
    Posts
    84
    Yes, there needs to be a "Z" value along with the "K" valure in the helical movement. K.0175 must also = Z-.0175. In other words, whatever your K value is, that is the value of your Z movement PER rotation. Thanks, John

  16. #16
    Join Date
    Aug 2005
    Posts
    197
    actualy,

    the "k" value is the lead like a thread pitch you can have a "Z-1" and a "k.2" and it will make 5 full turns to get to the programed " Z depth of -1"

    Did the drill portion work out?

  17. #17
    Join Date
    Sep 2005
    Posts
    84
    I didn't have any drill stuff to do today, maybe late Tuesday or Wednesday. The info you just gave me above is vary informative. WILL TRY THAT. I like that. So I just program in the final Z value, and the K is the "depth per rotation". Cool. Thanks, will try, John

  18. #18
    Join Date
    Aug 2005
    Posts
    197
    now you are cooking with gas as they say. Dont for get the full circle trick.

    Example Z-1 K.03 = BAD , it will not come out in the same place X&Y. The trick is to keep it even and unless you are cutting threads an extra turn will not take long.

    Z-1 K1. = 1 turn same start
    Z-1 k.5 = 2 turns same start
    Z-1.375 k.1375 = 10 turns same start

    I think you get it now so I will get of off the soap box and let you try it.
    John F.

  19. #19
    Join Date
    Sep 2005
    Posts
    84
    Thanks, I'm taking MANY notes. Thanks, John

  20. #20
    Join Date
    Aug 2005
    Posts
    197
    your welcome any time

    John F.

Page 1 of 3 123

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •