# Thread: Dynapath 20 Basic Programming question

1. 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.

2. Originally Posted by T0DD
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!

3. 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

4. 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!

5. 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

6. (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.

7. 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

8. 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.

9. Yes, a copy and past of what I sent to the machine this afternoon. I notice after it loads the Dyna-controller says *editing* before it is done. When I view the code it is slightly different than what I have posted above, but essentially the same. Machines fine, without errors, all the way down to line 45.

I noticed the sample posted by michaelthomas also has 2 gcodes on the first line N15:

(NMTB)
N15G70G90
N20E01T5M06(1 1/2 Face Mill)

Please excuse my basic questions, as I'm still pretty new to this. Should line 45 possibly be posting as a G2 or G3 event? Maybe I need to alter the post-processor in such a fashion? Looking at the part, this is when the first arc would begin I think, too. I am climb milling, CCW direction I believe. Also notice the S and M event together in line N30 of michael's sample and line N5 of mine...hmmm...

Program is for a simple 2" square pocket (ran fine) until I set corner radius to something other than zero (technically tool radius I suppose).

I'll plug away more tomorrow - just want to have some ammo to throw at it

Bill

10. I believe you are still in incremental on your arc moves, and the Dynapath is looking for Absolute. Hence the error message.

I don't do any Incremental programming, so it looks like Chinese to me.

11. Thanks Fighter -

In this line:

N47G3X1.175Y0.9125I0.0J0.025

EDIT: Found this:

I code = Absolute center of arc in x-axis
J code = Absolute center of arc in y-axis

and this:

The difference between programming in "Absolute" and "Incremental" is very simple on this control. All you do is add a "/" after the number you want to be Incremimental, and no "/" if you want absolute. This is in conversational mode which is what i use almost exclusivly, although you can mix "Regular" g-code in with it if you want.

Still googling...

12. The Absolute/Incremental setting that needs to be changed is in your CamBam
"Machining" folder. Set the "Arc Center Mode" to "Absolute" prior to generating G-code and then see if the controller still faults on arc moves.

If you are programming the Dynapath using G-Code, G90 and G91 set Absolute or Incremental mode. If programming using Conversational, you would use the "/" for Incremental.

You can't generate G-code in Incremental mode and have it run properly if the controller is in Absolute mode, which is what you seem to have done above.

They need to match or it will fault as it did.

Page 2 of 3 First 123 Last