New (to us) Brother TC-31A - and man do I have questions! - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 50
  1. #21
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    231
    Likes (Received)
    399

    Default

    Some folks on Practical Machinist were recommending this:

    Highland DNC, LLC.

    Shoplink flash. It's a USB adapter for your machine for about $229..

  2. #22
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Typing in the program may be an option depending on what I need to put in there.

    I was looking at a USB adapter on eBay but itís in Vietnam and would take a months to get here. That one could be here this week though..
    I donít mind using rs232, Iím already setup with that for our older wire edm and I had an AB switch box handy.

    Weíll see what today brings!

  3. #23
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    It Works! I can send and receive and the file compare says nothing bad happened in transit.
    For future reference if anyone has an A00 control and a null modem cable, the settings and wiring on this page worked for me:

    Brother TC-32 A G-code file transfer or DNC

  4. Likes Pete Deal liked this post
  5. #24
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Quote Originally Posted by Pete Deal View Post
    The BrotherComm software was something one of the Yamazen guys emailed me. Not sure it it was free back when it was the hot new thing or not. It's nothing fancy but works. As far as the pin connections being 2-2, 3-3, no this is not handled by the software. It depends on the equipment design and if each piece of equipment is a DTE or DCE. The terminology is sort of meaningless now since RS-232 became used for so many things over the years. Basically sometimes pin 2 can be transmit and sometimes it can be receive. Same with pin 3. This is what keeps RS-232 interfacing interesting. Hardware control is another issue. All I know is this works and it took me a few weeks of hair pulling to get it working.

    http://ftp1.digi.com/support/cabling/dte_vs_dce.pdf
    Someone told me once the good thing about standards is there are so many to choose from.

  6. #25
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    231
    Likes (Received)
    399

    Default

    Quote Originally Posted by Volitan View Post
    It Works! I can send and receive and the file compare says nothing bad happened in transit.
    For future reference if anyone has an A00 control and a null modem cable, the settings and wiring on this page worked for me:

    Brother TC-32 A G-code file transfer or DNC
    Excellent. I am sure that is a big relief for you.

  7. #26
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Quote Originally Posted by BROTHERFRANK View Post
    Excellent. I am sure that is a big relief for you.
    It is, thanks again for your relentless help on here.

  8. #27
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,713
    Post Thanks / Like
    Likes (Given)
    854
    Likes (Received)
    2555

    Default

    Quote Originally Posted by Volitan View Post
    Whoa I’ve never seen a cable like that before. Send and receive each going to each other?
    It's a 9 pin PC to 25 pin CNC cable set up to use hardware handshaking.

    For uploads and downloads with a CNC control's memory a 3 wire cable and software handshaking usually works fine. For drip feeding programs too large for the CNC memory I prefer to use hardware handshaking. IME, it is more reliable. Particularly when using a USB to RS232 converter.

  9. Likes Hardplates, Volitan, eaglemike liked this post
  10. #28
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,066
    Post Thanks / Like
    Likes (Given)
    549
    Likes (Received)
    421

    Default

    I have seen where people on here have said the calmotion boxes work too. I just bought a refurbished PC off ebay for $100+ which I think has more value since I can use it for other useful stuff in addition to downloading.

  11. Likes Volitan liked this post
  12. #29
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    I'm getting an error when I try to change tools in my program: 6207 Stroke Over Limit Z+
    If I change the tool manually then start thr program from that tool it works fine.
    We just ran a 3 tool job with short holders and no problems. These are slightly longer but not by a lot.

    After reading this thread: Z overtravel alarm on Brother Speedio
    I changed to using a G100. Here's the toolchange line with a few before it and after it

    Here's going from tool 1 to tool 2:

    G40 X-.6069
    G0
    G100 T2 G54 X-.7757 Y3.1413 S5000 M3
    G43 H2 Z.5 M8

    Tool 1 offset is 11.516
    Tool 2 is 11.2977

    In machine parameters I have:
    Stroke Z(-) .... 200.00
    If that means anything.

    Im missing something here

  13. #30
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    812
    Post Thanks / Like
    Likes (Given)
    1020
    Likes (Received)
    535

    Default

    Quote Originally Posted by Volitan View Post
    I'm getting an error when I try to change tools in my program: 6207 Stroke Over Limit Z+
    If I change the tool manually then start thr program from that tool it works fine.
    We just ran a 3 tool job with short holders and no problems. These are slightly longer but not by a lot.

    After reading this thread: Z overtravel alarm on Brother Speedio
    I changed to using a G100. Here's the toolchange line with a few before it and after it

    Here's going from tool 1 to tool 2:

    G40 X-.6069
    G0
    G100 T2 G54 X-.7757 Y3.1413 S5000 M3
    G43 H2 Z.5 M8

    Tool 1 offset is 11.516
    Tool 2 is 11.2977

    In machine parameters I have:
    Stroke Z(-) .... 200.00
    If that means anything.

    Im missing something here
    Might need a G90 in there, or at the beginning of the program.
    Also, what is your G54 Z value?

  14. #31
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Had a g90 and took it out.
    I have a .050 value in g54 z

  15. #32
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    812
    Post Thanks / Like
    Likes (Given)
    1020
    Likes (Received)
    535

    Default

    Quote Originally Posted by Volitan View Post
    Had a g90 and took it out.
    I have a .050 value in g54 z
    From here, I can't tell how you set up you parts, offset origin, etc.
    Is your tool offset number truly a positive number? Or did you forget to put a minus sign in there?

  16. #33
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    I know the tool heights are good because I can change to each tool in mdi and run the program from where itís called out and get a good part when itís done. Just canít change for some reason. I suspect itís a value in a parameter somewhere

  17. #34
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    231
    Likes (Received)
    399

    Default

    Two things to check/try. Are you running Z = zero in you work offsets? Try putting 5" or 6" in your Z work offset and subtracting the same amount from your tool offsets. Another thing is if you are calling G91 G28 Z0 anywhere, make sure it does not try to do it two times in a row. In other words, don't put it at the end of a tool and the beginning of the next tool. I think your issue is the tool lengths though, better to set the tools off of a gage block and get gage lengths and then set a Z work offset. I think max tool length on those machines is 7.87 inches. Tool and Work offsets are both positive when using G43 on Brother.

  18. Likes Volitan liked this post
  19. #35
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Quote Originally Posted by BROTHERFRANK View Post
    Two things to check/try. Are you running Z = zero in you work offsets? Try putting 5" or 6" in your Z work offset and subtracting the same amount from your tool offsets. Another thing is if you are calling G91 G28 Z0 anywhere, make sure it does not try to do it two times in a row. In other words, don't put it at the end of a tool and the beginning of the next tool. I think your issue is the tool lengths though, better to set the tools off of a gage block and get gage lengths and then set a Z work offset. I think max tool length on those machines is 7.87 inches. Tool and Work offsets are both positive when using G43 on Brother.
    I had a Zero Z in the work offset. I put 5" in there and subtracted it from the tools and it works.

    I'm using a 4" indicator height setter, and put 4" in the "Auto Tool Length Offset" parameter. So that was wrong? Should I put that to 0 and put the 4" in the work offset Z then?

  20. #36
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    231
    Likes (Received)
    399

    Default

    If you put the 4" in the auto tool length offset parameter and then when you set your tool lengths off that indicator using the auto set function in the tool data page with the indicator on the table not on the work, you will end up with the gage length for the tool offset. The tool length should be easy to visually check. if the tool is sticking out about 5" from the spindle your tool offset should be about 5". Then you will need to set the Z work offset. Take a tool that you know the length of touch the top of the work that you want to call Z0 and use the auto set function on the Z work offset. Then you need to subtract that known tool length from that Z work position. the machine can do it automatically but I can't explain it now I'm driving

  21. #37
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Quote Originally Posted by BROTHERFRANK View Post
    If you put the 4" in the auto tool length offset parameter and then when you set your tool lengths off that indicator using the auto set function in the tool data page with the indicator on the table not on the work, you will end up with the gage length for the tool offset. The tool length should be easy to visually check. if the tool is sticking out about 5" from the spindle your tool offset should be about 5". Then you will need to set the Z work offset. Take a tool that you know the length of touch the top of the work that you want to call Z0 and use the auto set function on the Z work offset. Then you need to subtract that known tool length from that Z work position. the machine can do it automatically but I can't explain it now I'm driving
    Thank you so much but yes, please don't do any of this while you're driving!

  22. #38
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    641
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    94

    Default

    Just looking through the manuals again to find out how to set up a job without manually entering numbers in work offsets etc..
    One of them says "See chapter 10 in the instruction manual"

    I've got 4 manuals. 2 programming manuals, an operation manual and an installation manual. Learned quite a few things from them but I think I'm missing one.

  23. #39
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    712
    Post Thanks / Like
    Likes (Given)
    231
    Likes (Received)
    399

    Default

    Ok. No way to avoid manually entering something for the Z work offset on the older A00 control machines unless you have a spindle probe I think. Machines older than 2003 need a software/hardware update to run probing macros too. For you, you can either take a cutting tool that you know the gage length of or you can use a special gage type tool that has a known length, say 5.000". To set the Z offset, touch the known length tool to the work piece zero, go to work offset Z in the Data Bank, hit Auto set, type in the known length in the Abs position after set field, (type in the # and hit Enter)the machine will do the math for you and subtract the tool length from the current Z machine position which will be your Z work offset. Save it, F0! The work offset is the height of the part from the table, the tool offset is the length the tool is sticking out of the spindle. Those two #s added together equals the machine position Z when the tool is touching Z zero on the part. When you add a tool setter, it will set gage length. When you add a spindle probe, it can set the Z (and X,Y) work offsets...
    Last edited by BROTHERFRANK; 12-14-2019 at 05:07 PM.

  24. #40
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,066
    Post Thanks / Like
    Likes (Given)
    549
    Likes (Received)
    421

    Default

    The way I do it is as follows-

    I have my tool setter height off the table set into the Switch 1 parameter "Auto Tool Length Offset". So if I was using the 3" length of a 123 block sitting on the table it would be 3".

    With the tool touching the setter (123 block in this case) I do the auto set for the tool length (TL Offset).

    My G54 Z zero is set to whatever distance my z zero is off the table surface. So say if my G54 Z=0 is the bed of my Orange vise, which is 3" high, then G54 Z would be 3.000.

    In practice I have a Haimer Taster that I keep in the machine as tool 99 and use that to measure my work offset Z. But the numbers work out as stated above.

  25. Likes Volitan liked this post

Tags for this Thread

Bookmarks

Posting Permissions

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