Dynapath 20 Basic Programming question

[wildwhl]

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

[gwiz]

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

[wildwhl]

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

[gwiz]

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.

[wildwhl]

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

[gwiz]

happy cutting

[rbickle]

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

[T0DD]

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

[rbickle]

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

[T0DD]

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

[rbickle]

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

[rbickle]

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