Dynapath 20 Basic Programming question


Page 1 of 2 12 LastLast
Results 1 to 20 of 31

Thread: Dynapath 20 Basic Programming question

  1. #1
    Member
    Join Date
    May 2010
    Location
    United States
    Posts
    327
    Downloads
    0
    Uploads
    0

    Default Dynapath 20 Basic Programming question

    Hello all. Made some progress today with the Tree VMC. Had some fun, and manually made some chips. Decided to give a go with conversational programming and ran into a ditch, of sorts.

    I can program tool, fixture, spindle, etc. - however - I cannot seem to select an event. What am I missing?

    For example, N0002 and I want to (0) position, or (1) linear mill and so forth - how is the (event) entered? I assumed I would simply hit next event, then (0) for position - then load coordinates - but I can't seem to have it accept anything other than M codes at this point. What am I missing?

    An example would be quite helpful.

    Thanks,

    Bill

    Similar Threads:


  2. #2
    Member
    Join Date
    Jan 2009
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    You must use the "EVENT TYPE" key. After you press the next event press the EVENT TYPE key to select the event you wish to program.

    Good day

    Gwiz



  3. #3
    Member
    Join Date
    May 2010
    Location
    United States
    Posts
    327
    Downloads
    0
    Uploads
    0

    Default

    Thanks gwiz - however - I'm still stumped. When I click event type it brings up another set of options: cavity mill, EIA, (forget what's next), setup, and text.

    I can enter text just fine - press T and enter text. To the left of those options are options 0-9 - and this is where arc mill, linear mill, etc. are. I can't seem to select those.

    So do I:

    1:Next event
    2:Event Type
    3:Cavity Mill? EIA? (which event type to I use to select arc, linear, etc)
    4:Then press the number that corresponds with the event I'm after?

    I've read the darn manual backwards and forward and I know I'm just overlooking it...

    Bill



  4. #4
    Member
    Join Date
    Jan 2009
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    Well, you should be able to press "EVENT TYPE" then select 0-9 or C, E,M,P, R,S,or T. These are all event types. Once selected it should bring up the corresponding screen listing the data location that can be filled in for that event.

    Other than that maybe I am missing part of your question. You can also check by using your text event to make sure the 0-9 keys are working.



  5. #5
    Member
    Join Date
    May 2010
    Location
    United States
    Posts
    327
    Downloads
    0
    Uploads
    0

    Default

    Somedays I think I'm losing my mind. I could swear I've done the exact sequence above dozens of times and never made it to the input parameters step. Booted the mill and tried it just now - shazam - it works.

    Thanks gain cnc'ers.

    WW



  6. #6
    Member
    Join Date
    Jan 2009
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    happy cutting



  7. #7
    Member
    Join Date
    Feb 2011
    Location
    USA
    Posts
    48
    Downloads
    0
    Uploads
    0

    Default

    Gentlemen,

    I have a Tree Journeyman 325 mill with the Dynapath Delta 20 controller. I've had the darn thing for almost a year now and am still trying to get it in service. The trouble is getting the CAM software with the appropriate post processor to work with the mill. I have several CNC machines using Mach3, but this one is very different.

    What CAM software / post processors are you all using?

    Thanks,
    Rick



  8. #8
    Member
    Join Date
    Jul 2010
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Default

    Greetings Rick-
    A slightly altered fanuc post will work (though there are a few stupid things).
    For arc center the vector is absolute arc center.
    Since the editor in the control is event driven, you cannot have two "G" commands in one line.
    For example, if you rapid Z to position and the call G1 G41 X1.0, that would be incorrect. Not a problem because you probably would have had the Z move as a feed move anyway, just want to point that out.
    As far as sequence numbers go, I increment by 1. If I have to insert a line at the control after N10, you could type N10.1
    Hope this helps!

    I'm using Unigraphics NX4, by the way.

    Todd



  9. #9
    Member
    Join Date
    Feb 2011
    Location
    USA
    Posts
    48
    Downloads
    0
    Uploads
    0

    Default Tree 325 with Dynapath Delta 20

    Todd,

    Thanks for the info.

    I've made it my priority this week to get the darn thing cutting something...

    I'm slowly figuring out the quirks of this controller - like no spaces whatsoever are allowed in the code.

    I'm running a test program and am getting an error on line 26.
    The error is Format Error 133, but I don't see what the problem is, can you help me out? Here is the first part of the code.

    (TSB2)$
    N0016(9)M06T1$
    N0018(0)G0Z0.1575$
    N0020(9)M03S6000$
    N0022(0)X0.0Y-0.1181$
    N0024(0)Z0.0197$
    N0026(1)Z-0.167F5.906$
    N0028(2)D0X-0.1181Y0.0Z-0.1673I0.0J0.0F5.9055$
    N0030(1)Y0.8661Z-0.167F5.906$

    Also, I have another question. Am I correct in assuming that when no tool Tx has been selected and no fixure Ex has been selected, that the machine will move position relative to the 0 point set by MODE, 0, 9? I have some programs that seem to move in absolute coordinates instead of moving relative to this point.

    Thanks,
    Rick



  10. #10
    Member
    Join Date
    Jul 2010
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Default

    Greetings Rick-
    Looks like the problem is on line 28 (D0).
    Lets cut a 2.000 X 3.000 block with a .250 radius on each corner using a 3/8" EM.
    X0Y0 is C/L of block, Z0 is top of block
    3.000 is along X axis, 2.000 is along Y axis.

    ---------
    (BLOCK)
    N1(T)10-26-2011$
    N2(T)1:10AM$
    N3(T).375-EM$
    N4T1M06
    N5S690M03
    N7(T)MILL-PERIMETER$
    N8G00X0.0Y-1.2875
    N9Z1.
    N10Z.1
    N11G01Z-.6F50.
    N12G41Y-1.1875F2.8
    N13X-1.25
    N14G17
    N15G02X-1.6875Y-.75I-1.25J-.75
    N16G01Y.75
    N17G02X-1.25Y1.1875I-1.25J.75
    N18G01X1.25
    N19G02X1.6875Y.75I1.25J.75
    N20G01Y-.75
    N21G02X1.25Y-1.1875I1.25J-.75
    N22G01X0.0
    N23G40Y-1.2875
    N24G00Z1.
    N25M30
    E
    ------------
    As far as fixture offsets, I've never used them. I do as you say and zero XY with "MODE,0,9". I've also not used the Z offset either yet, I just touch-off the tool and zero Z axis. I do use tool offset for cutter comp.

    Let me know!
    Todd

    Last edited by T0DD; 10-26-2011 at 09:47 AM.


  11. #11
    Member
    Join Date
    Feb 2011
    Location
    USA
    Posts
    48
    Downloads
    0
    Uploads
    0

    Default J325

    Todd,

    OK, great. Thanks for the info.

    Not sure why the CAM program was setting the tool diameter to 0 here.
    This brings up another point though. Cuter compensation.

    On my other routers using Mach3, the cutter compensation is controlled by the CAM software. The Delta 20 however, keeps a table of tool lengths and diameters internally and can compensate also.

    Do you typically program the tool parameters into the Delta 20 and generate G code with C1 and C2 parameters, or leave the Delta 20 tool diameters at 0 and have the CAM software calculate the offset?


    Thanks,
    Rick



  12. #12
    Member
    Join Date
    Feb 2011
    Location
    USA
    Posts
    48
    Downloads
    0
    Uploads
    0

    Default J325

    Todd,

    Another question: Upon studying your G code example, I see that you are using the EIA instead of the conversational format. What are the advantages / disadvantages of using each?

    Thus far, I have spent my time studying the conversational mode.

    Thanks,
    Rick



  13. #13
    Member
    Join Date
    Jul 2010
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Default

    Cutter comp is different on different controls. I almost always offset the tool path & use comp for adjustment only. If I'm thread milling I program online to geometry and comp for the tool size. An interesting thing to do is put a sharp felt marker in the spindle and cardboard, paper or whatever on the table and program a 4" diameter using comp. Bring Z down at the center of the arc and feed G41 X 2.0, cut a full diameter back to X2.0, G1 X0, G40. Run with no comp and you get a 4" diameter. Now run again with +1.0 comp & again with -1.0 comp. This Dynapath does some strange stuff. Some controls will enter and exit on Y0.0 with a straight line. This one only cuts 100% of the diameter with no comp, less than 100% with positive offset and more than 100% with negitive offset. Now on anyother control I would have all on one line:
    G1 G41 X2.0
    G03 X2.0 Y0.0 I-2.0 J0
    G40 G1 X0.0

    It is good to test like this so you can see exactly how the control handles things.

    As far as conversational goes I myself see no point in it. G-code can be run on any machine I have ever seen, you can learn it in about 300 seconds, and it is very easy to skip over sections, jump around in the program and such. It is very easy to scan with your eyeballs also. If the Dynapath was the only control you would ever use and you don't want to do much math then the conversational might be a good fit.



  14. #14
    Registered
    Join Date
    Nov 2007
    Location
    USA
    Posts
    90
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by T0DD View Post
    This one only cuts 100% of the diameter with no comp, less than 100% with positive offset and more than 100% with negitive offset.
    Hello Todd,

    Could you please clarify this a bit?

    If you program a 360 degree arc and it cuts less than 100% of it, how would you program it to do so.

    I'm not sure I understand what you are referring to here, as I use cutter comp and have never had a Dynapath cut an inside or outside diameter that did not cut 360 degrees of arc when programmed to do so. I use G-Code, not Conversational.

    If I program a 1" bore, I program the tool path for 1" and use comp to offset the tool by it's diameter. If the diameter ends up .999", I adjust the tool diameter in the tool table by .0005" so it cuts 1" diameter.

    I have never programmed an offset tool path and then used comp to adjust the cut diameter such as explained in the manual as "Negative Cutter Radius Compensation". If this is what you are referring to, I assumed it was to be used to make relatively small adjustments. 1" is a pretty large adjustment!

    Do you thread mill with the Dynapath?

    Thanks!

    Last edited by Fighter; 10-27-2011 at 08:23 AM.


  15. #15
    Member
    Join Date
    Jul 2010
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Default

    Greetings Fighter-
    I need to find a place to host photos and I'll upload one to show what I'm talking about regarding how comp acts on this control. I have not had to helical mill on the Dynapath yet, so I don't know if it will (G02 with Z move).
    Don't see any reason it wouldn't!

    Todd



  16. #16
    Registered
    Join Date
    Nov 2007
    Location
    USA
    Posts
    90
    Downloads
    0
    Uploads
    0

    Default

    Hello Todd,

    I re-read your post and believe I understand now what you are describing.

    I have not yet used the "Negative Cutter Radius Compensation", as it's referred to in the manual, but plan to play with that a bit this weekend. For a couple of years I wrote G-code programs on paper and then keyed them into the machine and always used regular Cutter Comp. I now have a second machine, and started using CAM and drip feeding or loading the program into memory via RS232. The CAM does not program with cutter comp, so I can put the "Negative Cutter Radius Compensation" to good use, which is what I believe you are doing.

    I have been using helical interpolation for plunging into different features and it works fine. I plan to purchase a thread mill and see how it works out. My CAM software doesn't do thread milling so I'll just manually program it to see how it works. I've looked at a couple of thread mill programs from thread mill manufacturers, but they mainly generate code for newer style Fanuc controllers, so it's not anything the Dynapath will digest without considerable editing. No synchronous spindles here, so it's a one pass deal.

    These Dynapath's seem a bit different compared to newer controllers, but seem extremely capable to me! I see comments as to them being unreliable, but all I have ever done is turn them on, and they run...(as long as the nit wit punching the buttons (me ) does everything correctly) so who knows!

    I learned a lot from your posts!

    Thank you!



  17. #17
    Member
    Join Date
    May 2010
    Location
    United States
    Posts
    327
    Downloads
    0
    Uploads
    0

    Default

    Finally had time today to play with the mill. Using CodeShark to edit files. Cambam to write them. Working on learning a lot in one day. Can successfully cut squares, but no arcs - errors at N45 - get Fault 021 start radius <> end radius. Surely I need to set something in CamBam Hopefully from this sample program somebody will help.

    Also - what is the syntax for naming a file for the Dynapath Delta controller?

    N1G20G90G64G40
    N2G0Z2.0
    N3T1M6
    N4G17
    N5M3S3000
    N6G0X0.425Y1.4875
    N7G1F25.0X0.575Z-0.05
    N8G1Y1.6375Z-0.1
    N9G1X0.425Z-0.15
    N10G1Y1.4875Z-0.2
    N11G1X0.575
    N12G1Y1.6375
    N13G1X0.425
    N14G1Y1.4875
    N15G1F10.0Y1.3875
    N16G1F25.0X0.675
    N17G1Y1.7375
    N18G1X0.325
    N19G1Y1.3875
    N20G1X0.425
    N21G1F10.0Y1.2875
    N22G1F25.0X0.775
    N23G1Y1.8375
    N24G1X0.225
    N25G1Y1.2875
    N26G1X0.425
    N27G1F10.0Y1.1875
    N28G1F25.0X0.875
    N29G1Y1.9375
    N30G1X0.125
    N31G1Y1.1875
    N32G1X0.425
    N33G1F10.0Y1.0875
    N34G1F25.0X0.975
    N35G1Y2.0375
    N36G1X0.025
    N37G1Y1.0875
    N38G1X0.425
    N39G1F10.0Y0.9875
    N40G1F25.0X1.075
    N41G1Y2.1375
    N42G1X-0.075
    N43G1Y0.9875
    N44G1X0.425
    N45G1F10.0Y0.8875
    N46G1F25.0X1.15
    N47G3X1.175Y0.9125I0.0J0.025
    N48G1Y2.2125
    N49G3X1.15Y2.2375I-0.025J0.0
    N50G1X-0.15
    N51G3X-0.175Y2.2125I0.0J-0.025
    N52G1Y0.9125
    N53G3X-0.15Y0.8875I0.025J0.0
    N54G1X0.425
    N55G1F10.0Y0.7875
    N56G1F25.0X1.15
    N57G3X1.275Y0.9125I0.0J0.125
    N58G1Y2.2125
    N59G3X1.15Y2.3375I-0.125J0.0
    N60G1X-0.15
    N61G3X-0.275Y2.2125I0.0J-0.125
    N62G1Y0.9125
    N63G3X-0.15Y0.7875I0.125J0.0
    N64G1X0.425
    N65G1F10.0Y0.6875
    N66G1F25.0X1.15
    N67G3X1.375Y0.9125I0.0J0.225
    N68G1Y2.2125
    N69G3X1.15Y2.4375I-0.225J0.0
    N70G1X-0.15
    N71G3X-0.375Y2.2125I0.0J-0.225
    N72G1Y0.9125
    N73G3X-0.15Y0.6875I0.225J0.0
    N74G1X0.425
    N75G0Z0.0
    N76M5
    E

    Thanks,

    Bill



  18. #18
    Registered
    Join Date
    May 2010
    Location
    USA
    Posts
    290
    Downloads
    0
    Uploads
    0

    Default

    (NMTB)
    N15G70G90
    N20E01T5M06(1 1/2 Face Mill)
    N25G94
    N30S1222M03
    N35G00X6.9376Y0.1933Z1.0F46.3
    N40G00Z0.1
    N45G01X6.9376Y0.1933Z-0.018F46.3
    N50G01X-0.75Y0.1933Z-0.018
    N55G00Z1.0
    N60G00X6.9376Y1.1366Z1.0
    N65G00Z0.1
    N70G01X6.9376Y1.1366Z-0.018F46.3
    N75G01X-0.75Y1.1366Z-0.018
    N80G00Z1.0
    N85G00X6.9376Y2.0799Z1.0
    N90G00Z0.1
    N95G01X6.9376Y2.0799Z-0.018F46.3
    N100G01X-0.75Y2.0799Z-0.018
    N105G00Z1.0
    N110G00X6.9376Y3.0232Z1.0
    N115G00Z0.1
    N120G01X6.9376Y3.0232Z-0.018F46.3
    N125G01X-0.75Y3.0232Z-0.018
    N130G00Z1.0
    N135E01T4M06(17/32 Jobber)
    N140G94
    N145S661M03
    N150G00X0.8247Y2.811Z1.0F7.2
    N155G00Z0.082
    N160G83R0.082K0.531Z-1.0436F7.2
    N165X0.8247
    N170Y0.811
    N175X1.8247Y2.811
    N180Y0.811
    N185G80
    N190G00Z1.0
    N195E01T3M06(3/16 High Helix Finisher)
    N200G94
    N205S5200M03
    N210G00X3.6407Y1.775Z1.0F7.3
    N215G00Z0.082
    N220G01X3.6407Y1.775Z-0.008F7.3
    N225G03X3.6407Y1.775Z-0.0525I3.7328J1.7927
    N230G03X3.6407Y1.775Z-0.097I3.7328J1.7927
    N235G03X3.6407Y1.775Z-0.1416I3.7328J1.7927
    N240G03X3.8249Y1.8104Z-0.1638I3.7328J1.7927
    N245G02X3.8281Y1.811I4.0134J0.829F14.6
    N250G02X3.8249Y1.8116I4.0134J2.7931
    N255G01X3.8246Y1.8116Z-0.1638
    N260G02X3.8214Y1.811I3.636J2.7931
    N265G02X3.8246Y1.8104I3.636J0.829
    N270G01X3.8249Y1.8104Z-0.1638
    N275G02X3.8693Y1.7942I3.8335J1.7652
    N280G03X3.913Y1.7762I3.9078J1.8255
    N285G02X4.1226Y1.7752I4.0134J0.829
    N290G03X4.1226Y1.8468I3.8247J1.811
    N295G02X3.8337Y1.8577I4.0134J2.7931
    N300G03X3.8158Y1.8577I3.8247J1.811
    N305G02X3.5269Y1.8468I3.636J2.7931
    N310G03X3.5269Y1.7752I3.8247J1.811
    N315G02X3.8158Y1.7644I3.636J0.829


    Here is a small excerpt from a program that runs fine on the Dynapath 20 I use. Maybe it will help figure out what is needed.

    The Program Name has to be in Parenthesis, must be all caps, and I think it can only be 8 digits......maybe 7......on the first line, too.



  19. #19
    Member
    Join Date
    May 2010
    Location
    United States
    Posts
    327
    Downloads
    0
    Uploads
    0

    Default

    Thank you for the response, michaelthomas. Not sure I'm smart enough to sort anything out from that though.

    Tested cutting a circle, and circular pocket and had the same error. Must be a setting in the post-processor stage? Currently have the ArcCenterMode property set to Absolute. Anybody out there have any tips?

    Bill



  20. #20
    Registered
    Join Date
    Nov 2007
    Location
    USA
    Posts
    90
    Downloads
    0
    Uploads
    0

    Default

    Is the code above exactly as you tried to run it?

    If so, it should have faulted on event N1.

    "N1G20G90G64G40"

    Only one G,M, S or T per event.

    Also event N45 is a linear event, so the error message you posted doesn't make sense. That message will only appear on a G2 or G3 event.



Page 1 of 2 12 LastLast

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

Dynapath 20 Basic Programming question

Dynapath 20 Basic Programming question