having trouble connecting bobcad and 8040m


Results 1 to 8 of 8

Thread: having trouble connecting bobcad and 8040m

  1. #1
    Registered
    Join Date
    Apr 2018
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default having trouble connecting bobcad and 8040m

    Howdy

    Was on the phone with the folks at bobcad ( mike , darren and cody ) and ( Yuli and Mohit ) Fagor canada . Bobcad guys are having a problem connecting predator to fagor with no results . After i downloaded windnc and got cody from bobcad on it we started to see some files arriving at cnc .
    Fagor canada has insisted that the part files be in 6 digit .pim format and we did that . Only some files ( not all ) would show up at cnc . Moreover , these files wouldn't run . First was a x axis ( softlimit ) alarm , Fagor said to take G54 out of the code & so I was presented with a y axis ( soft limit ) alarm after that .

    My knowledge of cnc is limited , my knowledge of cad/cam consists of 227 mind numbing bobcad/cam training videos , i understand the basics of electrical and plc and this is the first machine of 3 im trying to bring online in my garage .

    Too cheap to hire someone to do er , im getting the feeling that this is going to be a very educational experience .

    This being my first post , Id like to say hello ......the gentlemen at bobcad had alot of nice things to about this board




    heres the part bobcad sent
    %SCOTT TEST SQUARE.PI,MX--,
    N1 G90 G80 G70 G40 G17
    N2 G51E0.0893B45
    ;(Machine Setup - 1-Feature 2 Axis-Profile Finish)
    ;(FEATURE 2 AXIS)
    N3 T1
    N4 S3880 M03
    N5 G53
    N7 G00 X0. Y0.
    N8 G43 Z1. D1
    N9 M08
    N10 Z0.2
    N11 Z0.1
    N12 G01 Z-0.25 F22.3148
    N13 Y2.5 F44.6296
    N14 X2.5
    N15 Y0.
    N16 X0.
    N17 G00 Z0.2
    N18 Z-0.15
    N19 G01 Z-0.5 F22.3148
    N20 Y2.5 F44.6296
    N21 X2.5
    N22 Y0.
    N23 X0.
    N24 G00 Z0.2
    N25 Z-0.4
    N26 G01 Z-0.75 F22.3148
    N27 Y2.5 F44.6296
    N28 X2.5
    N29 Y0.
    N30 X0.
    N31 G00 Z0.2
    N32 Z-0.65
    N33 G01 Z-1. F22.3148
    N34 Y2.5 F44.6296
    N35 X2.5
    N36 Y0.
    N37 X0.
    N38 G00 Z0.2
    N39 Z1.
    N40 M09
    N41 M05
    N42 G0G53Z0
    N43 G0G53X0Y0
    N44 M30


    Im getting alarm 1155 x axis soft llimit over run . The fact that i zero my table in the center , try and run a part , return to the XYZ axis screen and values are back to " home position " zero values is troubling .

    any ideas ?

    There are some existing programs on fagor that were generated at HMI , those part programs work as they should without any alarms .

    thanks
    Regards
    Scott

    Similar Threads:


  2. #2
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    Quote Originally Posted by fairfieldmw View Post
    Howdy

    Was on the phone with the folks at bobcad ( mike , darren and cody ) and ( Yuli and Mohit ) Fagor canada . Bobcad guys are having a problem connecting predator to fagor with no results . After i downloaded windnc and got cody from bobcad on it we started to see some files arriving at cnc .
    Fagor canada has insisted that the part files be in 6 digit .pim format and we did that . Only some files ( not all ) would show up at cnc . Moreover , these files wouldn't run . First was a x axis ( softlimit ) alarm , Fagor said to take G54 out of the code & so I was presented with a y axis ( soft limit ) alarm after that .

    My knowledge of cnc is limited , my knowledge of cad/cam consists of 227 mind numbing bobcad/cam training videos , i understand the basics of electrical and plc and this is the first machine of 3 im trying to bring online in my garage .

    Too cheap to hire someone to do er , im getting the feeling that this is going to be a very educational experience .

    [COLOR=#000000][COLOR=#000000]This being my first post , Id like to say hello ......the gentlemen at bobcad had alot of nice things to about this board
    If you tried it like you posted, I don't think any control would like it, change what I have done and see if it helps


    heres the part bobcad sent

    %---------------------------------------------------------- ( SCOTT TEST SQUARE.PI,MX--, ) ( place like this in brackets, or remove altogether as I have done )
    (Machine Setup - 1-Feature 2 Axis-Profile Finish)--------------------( Move name to here, make sure there are only ) ( brackets used )
    N1 G90 G80 G70 G40 G17
    N2 G51E0.0893B45 ---------------------------- ( This may need to be in Brackets also ( G51E.0893B45 ) or removed if the control does not need it )
    N3 T1
    N4 S3880 M03
    N5 G53-------------------------------------------- ( Remove the G53 )
    N7 G00 X0. Y0. --------------------------------- ( This line also may need to be removed, G0 X0 Y0 this could be a crash waiting to happen, for a machining center you would not have this line in your program )
    N8 G43 Z1. D1
    N9 M08
    N10 Z0.2
    N11 Z0.1
    N12 G01 Z-0.25 F22.3148
    N13 Y2.5 F44.6296
    N14 X2.5
    N15 Y0.
    N16 X0.
    N17 G00 Z0.2
    N18 Z-0.15
    N19 G01 Z-0.5 F22.3148
    N20 Y2.5 F44.6296
    N21 X2.5
    N22 Y0.
    N23 X0.
    N24 G00 Z0.2
    N25 Z-0.4
    N26 G01 Z-0.75 F22.3148
    N27 Y2.5 F44.6296
    N28 X2.5
    N29 Y0.
    N30 X0.
    N31 G00 Z0.2
    N32 Z-0.65
    N33 G01 Z-1. F22.3148
    N34 Y2.5 F44.6296
    N35 X2.5
    N36 Y0.
    N37 X0.
    N38 G00 Z0.2
    N39 Z1.
    N40 M09
    N41 M05
    N42 G0Z0 ------------------ ( Remove the G53G0Z0 as I have done )
    N43 G53X0Y0--------------- ( You may have to remove the G53 here also, it will depend on your control, not all controls use G53 it can be used like G53 X0 Y0. by removing the G0 in )this line as I have )
    N44 M30
    %-------------------------------- ( Add % at end of program if you need it at the start then you need it at the end as well )

    Mactec54


  3. #3
    Registered
    Join Date
    Apr 2018
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    ive tried your suggestions and still getting alarm 1156 y soft limit over run N13 Y2.5 F44.6296

    thanks mactec



  4. #4
    Registered
    Join Date
    Apr 2018
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    https://www.cnczone.com/forums/fagor...-question.html

    i came across this thread late last night , can anyone please clarify what this means "Change your fixture offset inboard further and see if that works" .

    thanks



  5. #5
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    Quote Originally Posted by fairfieldmw View Post
    https://www.cnczone.com/forums/fagor...-question.html

    i came across this thread late last night , can anyone please clarify what this means "Change your fixture offset inboard further and see if that works" .

    thanks
    Post the program that will run, you can check where your soft limits, by moving each axes to the max travel, you can only do this after homing the machine

    So first test Home your machine and then move the axes around to the max travel it will go, if each axes moves to the machines max travel then you don't have to change anything with the soft limits in the control

    The fault is showing that your part position is outside the soft limits

    In your Cad program check where you X0 Y0 is on your part, for normal milling you have the X0 Y0 at the top left hand corner, but can be anywhere on the part, as long as you know where

    So in your machine you have to set your work off set Part X0 Y0 this position would be saved in the work Off-Set Page in the Control and would be a G54 which I don't see in your program

    In the work Off-Set page you set your work X0 and Y0, this has to match where it is in your drawing this will be your G54 Off-Set, and should stop you Fault you are having if you have this set correct

    The other thing to look at is what is your machine set in Inches or Metric, this to can cause the same problem, as what you are having, but I suspect your work X0 Y0 is not set correct

    You have a G70 in the header which is telling the machine control that your program is in Inches, it would be a G71 for this control if your program was in Metric

    N1G90 G80 G70 G40 G17
    G54---------Add and set your work off set to match your drawing X0 Y0 position

    Mactec54


  6. #6
    Registered
    Join Date
    Apr 2018
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    Right on ,

    Thanks for following up buds , but Im having no such luck . Maybe im missing something

    - I homed machine and then jogged each axes till a travel alarm came up

    - Jogged table to a central location , zeroed xyz screen and the zeroed all axes at G54 offset page

    - Cam file looks pretty close to zero

    - both cam and cnc are working in inches

    I now notice that part programs generated at hmi that would simulate before but now throw a soft limit alarm . The instant i push start , my xyz zero reverts back to machine coordinates

    regards
    Scott

    Attached Thumbnails Attached Thumbnails having trouble connecting bobcad and 8040m-20180430_061335-jpg   having trouble connecting bobcad and 8040m-20180430_061240-jpg   having trouble connecting bobcad and 8040m-20180430_061103-jpg  


  7. #7
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    Quote Originally Posted by fairfieldmw View Post
    Right on ,

    Thanks for following up buds , but Im having no such luck . Maybe im missing something

    - I homed machine and then jogged each axes till a travel alarm came up

    - Jogged table to a central location , zeroed xyz screen and the zeroed all axes at G54 offset page

    - Cam file looks pretty close to zero

    - both cam and cnc are working in inches

    I now notice that part programs generated at hmi that would simulate before but now throw a soft limit alarm . The instant i push start , my xyz zero reverts back to machine coordinates

    regards
    Scott
    Yes you are not doing your X0 Y0 correct, they would not have a zero

    When you Home the machine that is the machine Zero positioning anywhere away from these home positions will have a number, your work will never be at a Zero point

    So G54 would have a Number from the machine Home point to the X value and a Y value to where ever you have your X0 Y0 on your work piece

    Your machine may Home in a different direction than this, but the same thing applies the G54 will have numbers where ever your work is placed

    Attached Thumbnails Attached Thumbnails having trouble connecting bobcad and 8040m-work-offsets-basic-png  
    Mactec54


  8. #8
    Registered
    Join Date
    Apr 2018
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: having trouble connecting bobcad and 8040m

    awesome ,

    simple , duh ......thanks a bunch fella



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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

having trouble connecting bobcad and 8040m

having trouble connecting bobcad and 8040m