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
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:
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
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
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.
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
happy cutting
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
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
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
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.
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
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
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.
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.
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
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!
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
(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.
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
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.