584,849 active members*
3,889 visitors online*
Register for free
Login
Page 2 of 3 123
Results 21 to 40 of 49
  1. #21
    Join Date
    Mar 2019
    Posts
    94

    Fanuc series 21-M

    They found the manuals, where I bought the machine. I was also communicating with Fanuc, they took some numbers off the back and said I have a 20-MA control. I also got detailed instructions on how to back everything up which many have advised I do, my cable should be here today.


    Sent from my iPhone using Tapatalk

  2. #22

    Re: Fanuc series 21-M

    Great news. You are now totally set. Let me suggest that Peter Smid CNC programming book once again. Even though it's full of details and just about everything you'll ever want to know about programming a Fanuc control, it's written more in layman's terms or CNC for Dummies kind of thing. The Faunc books and even some Programing Manuals supplied by the manufacturers can be a tough read sometimes. Especially for a beginner. Though the factory manuals will give you an idea of what options and functions are available to you. Mostly applicable M and G codes.

    Try to at least download off the internet a Fanuc 20MA Operations Manual, Parameter Manual and Programming Manual if you can find them. Look for the ones with the highest revision number. Usually a slash/ with a number at the end. These manuals will touch on things that may not be described fully in the books that come with the machine. Likely the programming is going to need your most attention. That machine of yours looks like it's ready to run without trouble for a long time.

    May I suggest ER type Collet Chucks for the bulk of your tooling. They're very common and used by a lot of people both pro and beginner. Many manufactures have startup kits were you can buy a bunch at reduced cost. Try maybe ER16 or ER20 for the smaller stuff and ER32 for the rest up to 3/4". Above 3/4" you can stick with End Mill Holders although it doesn't hurt to have at least one of each down to say 3/8". I would stay away from using drill chucks unless you get those designed for CNC machines which tend to have hard braking spindles. Your average drill chuck is not designed for that. Pay attention to the pull stud (retention stud) on the back of the tool holders. Your machine will only accept one type out of all the types out there. Get to know your pull studs style and dimensions should you ever need to get more. You do not want to use the wrong one.

    I'd better get back to work. Have fun...

  3. #23
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    Got Um




    Sent from my iPhone using Tapatalk

  4. #24
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    Lot of info here. Been searching an atc alarm 20, checked the sensors, all good manual says to check the counter value set in PMC data # 1845. Says to change the value of the magazine position counter #1845 to the position number currently indexed if not right.

    How do I get into pmc 1845 to check this?

    Thanks
    Craig


    Sent from my iPhone using Tapatalk

  5. #25

    Re: Fanuc series 21-M

    Hello Craig,

    It's likely on your System screen then push PMC then DATA. Not exactly sure how your screen plays out. If you want to change something you have to go to the Offset Screen and set PWE to 1. (Parameter Write Enable) and also be in MDI mode. (It will throw an alarm but that is normal. Once you turn it back to 0 and hit RESET it will go away.) Usually you can type in a parameter number then hit some Search (SRCH) soft key to get you there. Watch your buffer area on the screen when you're typing.

    Your best bet is your Fanuc or Miyano Operations Manual. In that book it will show you how to get through and to every possible screen page the control has. Mine as well get use to that book right from the start as you'll find it useful many times until you start getting the hang of it.

    I was just looking at a downloaded version of your 21MB Operations manual B–62704EN/03 I got online. Go to section 2.3 and start there. In a few pages you/ll get to the SYSTEM and OFFSET/SETTING screens which are where all the control controlling stuff is. In one way or another, this one book will tell you how to do just about everything on how to work through the control and do things, including looking at or changing parameters.

    Hope you got your parameters backed up.

    I don't mind helping at all, but I can't promise I'll always notice you've asked a question. Especially if I'm busy in the shop.

    ADDED: Your DATA tables and KEEP RELAYS and TIMERS settings and things like that are usually listed with descriptions at the rear of your Ladder Manual if you have one. Data tables are generally areas of the control that store stuff like Machine State when last turned off, things like that. Keep Relays too. If that PMC DATA 1845 is a Data number, understand it will have a different meaning and be in a different place in the control then you Parameters. You will also most likely have a Parameter 1845. Actually 1845 seems high for a DATA number but I'm just going off of my memory which isn't always the best.

    Dave

  6. #26
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    I’m in no hurry. It showed tool 7 and tool 8 was at the spindle, I’ll try it now, thanks


    Sent from my iPhone using Tapatalk

  7. #27

    Re: Fanuc series 21-M

    It's typical for a control to have the the tools in the Tool Carousel described in the DATA Tables. There may be info in your book as it seems you found some already. The information about which tool is in which pot and which is in the Spindle will all be there grouped together. Most machines have Random Tool capabilities, meaning Tool Pot 1 will not necessarily have Tool1 as described in your Program in it. Meaning any numbered tool in your program can reside in any numbered Tool Pot on the machine. Hope that makes sense.

    You might have to watch out when changing active tool numbers that you don't end up with doubles. If you're lucky your Data info will be in standard form where a 6 is a 6 and so on. Some times this info is in Byte or BIN (Binary) or HEX (Hexadecimal) form. There are BIN to Hex to Decimal convertors you can find online that can help make sense of these computer type numbers.

    Example

    Decimal 16

    Hex 10

    Binary 00010000

  8. #28
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    I’m getting there one issue at a time, the spindle now starts up, previous programs run, go through the tool changer and select the correct tool, issue right now is the over travels.


    Sent from my iPhone using Tapatalk

  9. #29

    Re: Fanuc series 21-M

    If those existing programs you're running are over traveling, it's only because the work offsets are not set correctly for them. Look in the program for a work offset call. (G54 thru G59) Then look at your OFFSET/Work soft key screen and see what is in there for whatever offset is called in the program. You will have to do the following to stay out of over travel range. You have a small Work Envelope so that is part of the reason why you're fighting it.

    If G54 is the work offset in your program.

    G54 X will need to be a negative number equal to or slightly larger then the largest positive X value you find in the program. (If there are negative X, see below about Y) If all your programmed X values are Negative which is doubtful, you will have to set a work offset that combined with the largest Negative number, is still less then the total available travel of your machine in the X axis.

    For instance. Say your maximum machine travels are X 20" and Y 14". That is your 2D XY plain Work Envelope. Say the largest X coordinate you find is X12.25. Set your G54 X anywhere between X-12.35 and X-19.9. That will keep you from over traveling in X. (Assuming there are no negative X values.)

    Y is the same. I'll use a negative this time. Say the largest negative Y value in the program is Y-5.375 and the largest positive value is Y3.0. That means you have an 8.375" total Y axis movement to worry about. As long as you set your G54 Y to at least Y-3.1, but no more then Y-8.525 you should not over travel the machine. Following that?

    These are not scenarios you will typically even need to concern yourself with when running your own programs. You will mount your vise to the machine bed. Load your raw stock. Locate the corner or center of your stock using an Edge Finder or Dial Test Indicator if locating a Bore or round stock, look at the numbers you then see on the Machine Coordinates Screen, and enter those numbers in your G54 Work Offset. Then you're ready to go... carefully at first.

    The above presumes that the entire programs you're trying to run in are completely done in Absolute Mode (G90) (Pretty typical) If you find X and Y coordinates coming after a G91 (Incremental Mode) but before another G90, they are Incremental moves. Meaning they represent a move distance and not a move to a coordinate relating to anything like your Work offset or even Machine Zero.

    Finally - Work and Tool Offsets will always be negative numbers. You should see a G43 near the beginning of each tool in the programs you have. There will be an H number next to or very near the G43 including a Z value of possibly Z0.1 or something. G43 is what calls the Tool Offset H. Example. G43 H6 tells the machine to go to the Tool Offset Register and use the number it finds in Register 6 as the height of the tool coming into play. Now the machine knows what it's dealing with.

    Okay... I really do have to get to work. It's already after lunch. Hope this gets those programs running for you. If it works from start to finish without problems, run it at Full Rapid and see what your machine has for speed. Should be fun.

  10. #30
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    I have everything backed up has to do a little rewiring of the cable then worked great. I’m using DNC4U software


    Sent from my iPhone using Tapatalk

  11. #31

    Re: Fanuc series 21-M

    Sounds great Craig. Meaning to ask. Do you have manual machining experience?

    Here is a sample of one program with spotting, drilling, tapping and one end mill. It's not complete as it was for doing 8 parts in multiple vises and I simplified it down to one place and deleted a bunch of stuff to keep it short. Not meant to be run but only as a Programming Format Example. All my programs look like this or some version of. I program manually with CAM aid. BobCAD 20. You might end up using the BobCAD post processor in your software. Personally I find a lot of what I see post processors spitting out is junk. Not sure you'd could manipulate your processor to look like this or not.

    The explanations in color are just that. If you copy and paste this into a text file and delete all the colored text it will give you a better picture of what the program looks like. I like having the header at the beginning of each tool as it makes it easier to find things as you're speed scrolling down a page.

    Just food for thought. Sound like your machine is ready to make parts.

    SAMPLE ONLY

    %
    O2033(LARGE PADDLES)

    (T1 SPOT DRILL 120 DEG)
    (T2 13/64 DRILL 118 DEG)
    (T5 17/64 DRILL 118 DEG)
    (T15 3/32 2FL END MILL)
    (T16 1/4-20 SP TAPPER)

    (PROGRAM ZERO IS FIXED JAW)
    (AND LEFT EDGE)
    (Z ZERO IS TOP OF PART)

    (USING ONE TWIN VISE)

    T1M6 (SPOT DRILL) - Tool Call and Name
    G17G20G40G49G54G80G90G98 - Safety Line. Makes sure machine is setup in known safe condition before every tool. (Explanation at end)

    G0X0.3125Y4.6654 - Move to first position while head is safe at tool change position.
    G43Z0.1H1S3500M3 - Move to Initial Plain, Call tool length offset and start CW spindle at speed.
    M8 - Turn on coolant while head is down at part. (No mess) On single line so with Single Block Active gives chance to adjust coolant nozzle(s)
    G99G82Z-0.064R0.1P50F21. - Spot Drill Cycle (G82 - Drilling with Dwell)(G99 Return to R Level in Fixed Cycle)(P dwell in milliseconds)
    Y3.6654 - 2nd position etc.
    Y2.6654
    X1.3125Z-0.077 - Can change any parameter from line (G99G82) above during fixed cycle without canceling first.
    X2.3125Z-0.064 - Changed Z level back again on next hole. Spotting with chamfer on what will be two different hole sizes.
    Y3.6654
    Y4.6654
    X3.0625
    Y3.6654
    Y2.6654
    G80 - Cancel Fixed Cycle
    M9 - Coolant off

    T5M6(17/64 DRILL)
    G17G20G40G49G54G80G90G98

    G0X1.3125Y4.6654
    G43Z0.1H5S2792M3
    M8
    G99G81Z-0.455R0.1F17. -(G81 Fixed (Canned) Cycle. Drilling without Dwell)
    X4.0625
    Y-0.5
    X1.3125
    G80
    M9

    T2M6(13/64 DRILL)
    G17G20G40G49G54G80G90G98

    G0X0.3125Y4.6654
    G43Z0.1H2S3575M3
    M8
    G99G81Z-0.386R0.1F21.4
    Y3.6654
    Y2.6654
    X1.3125
    X2.3125
    Y3.6654
    Y4.6654
    X3.0625
    Y3.6654
    Y2.6654
    G80
    M9

    T16M6(1/4-20 TAPPER)
    G17G20G40G49G54G80G90G98

    G0X1.3125Y2.6654
    G43Z0.3H16S350M3
    M8
    G99G84Z-0.5R0.3F17.5 - G84 Tapping Mode. Notice the Feed divided by the Spindle Speed equals the Lead of the thread. (0.050") This machine does not have Rigid Tap. Using Tension/Compression Holder and added clearance height to give machine time to get up to speed. (Z0.3 instead of normal Z0.1)
    X4.0625
    Y-2.5
    X1.3125
    G80
    M9

    T15M6(5/32 END MILL)
    G17G20G40G49G54G80G90G98

    G0X0.0918Y0.1
    G43Z0.1H15S5500M3 (machine has 6000 max spindle. seldom run it there even as I could with this tool.)
    M8
    G1Z-0.06F16.5 - Move to cutting depth
    X0.8008Y-0.6874
    Y-0.7875
    X-0.1
    G0Y-2.2125
    G1X0.8008
    G0Z0.1
    X-0.1Y-2.5497
    Z-0.06
    G1X0.935Y-3.1
    G0X1.69

    etc-etc-etc

    X1.8242
    Y4.478
    X2.5332Y5.2654
    G0X0.0918
    G1X0.8008Y4.478
    Y4.3779
    X-0.1
    G0Z1.
    M9
    G53Z0.Y0.M5 - Return Head to Zero (Home) Position and bring table full forward to reload using G53. Do not use G28. Also stopping Spindle while heading home.
    M30 - Program end w/ Rewind back to head of program
    %

    Note another highly useful tool is G98 in a Fixed Cycle. This allows you to jump over obstacles in the way of your drill movements. G98 is Return to INITIAL Level in a Fixed Cycle, whereas G99 is Return to R level in a Fixed Cycle. Say you have some clamps that are 2" tall holding down your work. I'll grab a tool from above and change it to jump over obstacles.

    Jumping over obstacles with G98

    T2M6(13/64 DRILL)
    G17G20G40G49G54G80G90G98

    G0X0.3125Y4.6654
    G43Z2.5H2S3575M3 - This position in all the tools above is your Initial Plain. Whatever the Z axis height is when a Fixed Cycle is called is your Initial Plain. "R" is the height that ALL drilling cycles start their work from. (R Level) If you jump over an obstacle, the drill will rapid back to R height (here R0.1) before its starts drilling. Meaning in this case it will not start drilling from 2.5 inches above the part that you went to when jumping over the obstacle. After raising up and jumping over, it will rapid back to R and start working from there. G98 is also useful for getting down quickly into deep holes, but you have enough here already.
    M8
    G99G81Z-0.386R0.1F21.4 - Starting out Retracting to R Plain (0.1)
    Y3.6654
    Y2.6654
    G98X1.3125 - After drilling this hole it will retract to Z2.5" before moving to the next hole. Here is you jumping over an obstacle. But it will Rapid to R before starting work.
    G99X2.3125 - After this hole it will again retract to R level (R0.1) and move to the next hole right above the work.
    Y3.6654
    Y4.6654
    G98X3.0625 - Jumping over another obstacle with G98 Retract to Initial Level in a Fixed Cycle
    G99Y3.6654 - And again returning to G99 Retract to R level in a Fixed Cycle.
    Y2.6654
    G80
    M9

    Hope this helps. It's all in the Smid book I mentioned. After deleting all the brown writing in the single tool example above, you should be able to run this above your table to see what I mean.

    Almost forgot. Safety Line

    G17 - X Y Plain Select
    G20 - Imperial units (Inches)
    G40 - Cancel Cutter Compensation
    G49 - Cancel Tool Height Offset
    G54 - Initiate G54 Work Offset
    G80 - Cancel Fixed Cycles
    G90 - Absolute Positioning Mode
    G98 - Retract to Initial Level in A Fixed Cycle

    Have fun learning.

    Dave

  12. #32

    Re: Fanuc series 21-M

    One last thought. The above program happens to have the Initial Plain and the R Plain at the same height in all the tools. Being Z0.1" in both (G43Z0.1) and (R0.1) . In these cases G98 and G99 would act the same and either one could be used.

    Here is one last example of using G98 in the opposite direction of what was shown above. Instead of jumping over an obstacle we're going to jump down a hole that was drilled earlier with a larger drill. Meaning you have a two diameter hole with a step in it.

    Let's say a previous drill that was a little larger then the one following here has already drilled 1" deep in all locations.

    T2M6(13/64 DRILL)
    G17G20G40G49G54G80G90G98

    G0X0.3125Y4.6654
    G43Z0.1H2S3575M3 - Back to normal Initial Height
    M8
    G98G81Z-1.75R-0.9F21.4 - Again Retract to Initial Level in a Fixed Cycle. Then regardless of what a drill is doing getting to a hole, meaning whether it comes form on high or is skirting right over the material at Z0.1, it will always Rapid to R Level. So in the scenario your drill will run around the part at Z0.1 above the stock, but right before drilling each pre-drilled hole, it will Rapid down the existing hole to 0.1 above where the previous drill left off. (Z-0.9) That way no wasted time drilling air for a full inch. (1.10" actual.)

    Y3.6654
    Y2.6654
    G80
    M9

    Dave

  13. #33
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    I might be jumping ahead but I’m waiting for my new linear rails and bearing blocks for XY a bit rusty from sitting so long.

    Anyhow this machine now zero returns to -X and -Y. I want to start from zero being +X and +Y so any offset will be in the plus direction except for Z which will be minus.

    Any ideas or is this a dumb idea? This is how my Denford mill is setup in mach3 so it’s like looking at my cad program with the axis shown in the lower left corner.


    Sent from my iPhone using Tapatalk

  14. #34

    Re: Fanuc series 21-M

    Wow - replacing rails is serious and precision work. I hope you have the measuring equipment to verify your installation. Including tenth reading indicators at a minimum. It will help some that your machine has a small-ish work envelope. I've done it myself once and it was serious and sensitive work. I wish you luck on that job. A little tip, completely level and square up your machine before you start tearing it apart. You'll want it there for when you're putting it back together again.

    I've never seen a machine go anywhere when homing except to the upper right corner of the table. Meaning all offsets will be negative. Maybe some do but I've never seen one. Could be all my machines are from Japan and Taiwan. I'm not sure you could do what you're after unless you swapped out all the trip dogs mounted on the sides of the table and saddle. Likely have to move all the switches too. These devices control the homing of your machine. Also don't know if your ladder logic would except that change or not.

    Not sure what you're hoping to gain short of keeping it like the other machine. There is still nothing keeping you from programming all your work to the lower left corner so all the coordinates in the program are positive, but this is not the way to go in many cases. At least not in those cases involving a vise for work holding. The fixed jaw of the vise needs to be your Y zero. Only the fixed jaw is a repeatable stop. Unless you want to mount your vises with the handle to the rear which wouldn't be very handy, I think you're stuck like the rest of us with Y zero being the top of your part when viewing in CAD. If you mount your vises sideways then you could make the lower left corner X0Y0., but that doesn't seem practical either.

    I believe Kurt and maybe others sell a reverse acting vise where the fixed jaw is toward the operator. You might pay a little more and be less likely to find these things at auction or on eBay, but if that's what you're really after that would be a way to go. Truth is your CAM is going to be spitting out all your coordinates anyway. What does it matter if they have negative signs mixed in with them? Also there's likely functionality built into your machine that is going to enter Work Offsets or Current Positions into Work offsets for you anyway. Meaning it's possible you won't be typing them in by hand to begin with.

    It's your shop and show so do as you please for sure. I personally don't see the need. But that's not your problem.

    After all the rail replacements are done, you might want to spend the money and have the machine Ball Bar Tested and Laser Calibrated. This will give you a full folder of information about the movements of your machine and they'll also give you the Pitch Error Compensation and Backlash numbers to enter into your control to counteract errors in the movements of your screws. Well worth the cost and the peace of mind from knowing.

    Good luck with that rebuild. Get yourself a Hard Arkansas stone for prepping the mounting surfaces. I'll lay off the programming ideas. Sounds like you won't be needing any for awhile.

  15. #35
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    This is my first machine with rails and bearing blocks. My history is rebuilding manual mills and surface grinders, Bridgeport’s and Parker Majestic scraping ways, grinding gibs etc, lot of work and time but with the right equipment I’ll shoot for one to two tenths


    Sent from my iPhone using Tapatalk

  16. #36

    Re: Fanuc series 21-M

    Well shoot... you hardly need me yapping at you.

  17. #37
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    I’m leaving the home or zero where it’s at, reading thru what you said makes sense plus probably can’t change it anyhow. I got enough learning to do besides screwing with a machine that’s mostly setup already.


    Sent from my iPhone using Tapatalk

  18. #38
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M




    Sent from my iPhone using Tapatalk

  19. #39
    Join Date
    Mar 2019
    Posts
    94

    Re: Fanuc series 21-M

    Alright experts! I’m stumped. Can’t find much about memory in the manuals. On the controller is a slot. The card slot says CNMC memory and it’s empty.

    Can I add memory to this?

    Thanks


    Sent from my iPhone using Tapatalk

  20. #40
    Join Date
    Dec 2009
    Posts
    947

    Re: Fanuc series 21-M

    that CNMC slot is for an SRAM CARD used for back-up the controller not for memory extension.
    what you want to do?

Page 2 of 3 123

Similar Threads

  1. Replies: 5
    Last Post: 04-20-2019, 02:31 PM
  2. Replies: 4
    Last Post: 02-21-2019, 08:24 PM
  3. Fanuc Series
    By Khanfirovic in forum Fanuc
    Replies: 0
    Last Post: 09-25-2018, 11:42 AM
  4. Replies: 28
    Last Post: 05-21-2015, 12:35 AM
  5. FANUC Series 18-M
    By Kristoffersen in forum Fanuc
    Replies: 2
    Last Post: 01-16-2009, 11:17 PM

Tags for this Thread

Posting Permissions

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