BACKPLOT vs POSTED NC CODE

[M. Anderson]

First off - Thanks, to everyone who has tried to help me with all my problems. This place is great, the wealth of knowledge here is astounding!

 

Now, the questions -

 

Q #1. Do most of you who program the machines use the backplot function in MC?

 

Q #2. Do you not expect the posted *.NC code to match the backplot? Move for move?

 

Q #3. When drilling a series of holes - should the posted *.NC output, not return to the input (EDIT) "Clearance Height", if selected, before moving to the next drill location?

 

EX: if I set the (EDIT)"Clearance Height", to 1" should the posted code not return to 1" above the part before moving between the points? Currently the post outputs this position at the start of the drilling and at the very end.

 

Q #4. This control seems to be reading "Cutter Comp (G40/C0) - Off", codes 2 lines ahead of when it should actually turn the CC off. Any ideas on how to fix this?

 

Again- THANKS FOR ALL YOUR HELP!!! Everyone!

 

Let me know where to send the BEER!

 

Mark

 

(EDIT - I had said "retract height" above and ment "Clearance Height")

 

[ 03-03-2003, 10:25 PM: Message edited by: M. Anderson ]

[Scott Bond]

Hi

 

 

Q #1. I use the the MC verify ,and once in a while the backplot feature

Q #2. I expect the posted *.NC code to match the backplot Move for move.(with my familer post)

Q #3. When drilling a series of holes - I expect to have full control over the tool.

Q #4. I am not the guy for this one.

 

[ 03-03-2003, 09:04 PM: Message edited by: Scott Bond ]

[Guest CNC Apps Guy 1]

Hello,

 

Q1: I use backplot when I want to check tool motion. I use verify essentially to check the end result.

 

Q2: I would venture to say yes, but to tell you honestly, I've never checked.

 

Q3: In V9 you have the option to select weather it returns to clearance height before proceeding to the next position or only going to the clearance height in the first position and the last position. SO the answer as I see it is yes and no.

 

Q4: Is it possible your control has some sort of look-ahead function and is actually looking ahead and executing prematurely? BTW, what type of control is it?

 

HTH

[chris m]

Q #1. Yes, along with verify

 

Q #2. Yes; as long as: 1) the machine is physically capable of making the moves you are programming 2) the post is reliable and proven for the machine

 

Q #3. If I tell the machine that I want that; ie G98, then that's what I'd expect

 

Q #4. The control shouldn't read a G40 until there is a G40; do you mean that the post is outputting G40 "early"? If so, you might want to add a small lead-out line. If not, it may be some kind of look-ahead issue, as James said.

 

C

 

[ 03-04-2003, 07:16 AM: Message edited by: chris m ]

[M. Anderson]

James - It is a Dynapath Delta 20 control.

 

And, Yes, I do think it is some kind of "look-ahead" that is happening.

 

But has anyone ever heard of something like this? It don't make sense for CC to be read in before the line it is coded on, and canceled while still making a cut on a line 2 lines before it should be turned off?

 

I use backplot too check the motion of the tool, it gives X,Y,Z moves at bottom of screen, then use verify too see part.

 

Chris - the machine is capable of making the moves - the post is just not out-putting the correct code?

 

And I am using lead in and lead out moves - but the CC-off (G40), is being picked up and executed before the line it is on is even executed? I think James is right - somekind of look-ahead - but I cannot find how to turn it off!

 

V9 may work better - but currently I am stuck using V8.1. I am just trying to get the post straightened out for this machine, going too try my dealer again! Mabey I can make him understand the problems better this time?

 

Thanks everyone,

 

Mark

[McRae]

Do not output the G40 until the tool has retracted - For those of us who had used a Fanuc7M, we can sympathize.

[Charles Davis]

The G40 problem can definitely be solved with tweaks to the post. Turning comp off after the tool has retracted is difficult, not impossible, but difficult.

 

I highly recommend a short lead out line to turn off cutter comp instead.

 

You need someone who really knows the post to work on this one.

[Surface]

I love that control with a couple exeptions. Cutter comp is one of them. Dynapath institutes the cutter com after the first move and before the last move. Therefore, if you are using cutter-comp in the control, I recomend you use both entry/exit lines and arcs. This will get the cutter-comp move after the liniar move, but before the arc move.

I don't think this control can use negitive tool diameters, so for tweaking-in wear-comp, Somtimes I would program with a .24 dia cutter, cutter-comp computer and wear-comp, and leave the cutter comp in the control at .01 (1/4 dia endmill.

[chris m]

General question:

 

Would using an "exact stop" command where this cutter comp issue is occurring stop it?

 

If the machine could be forced to execute the entire block before reading the next, this would reduce the occurrence of this problem; or would it?

 

C

 

[ 03-04-2003, 11:37 AM: Message edited by: chris m ]

[mmonica]

I, too, like the Dynapath control. You will not be able to get canned cycles (drilling, boring, ect) to jump like a Fanuc using G98, G99. You must cancel the canned cycle using a G0 Z move and start another group of holes. This is a control issue, not a MasterCam issue. My Dynapath 20 will not accept a negitive cutter comp value, what I have done in the past is to change the C1 to a C2 or C2 to a C1. My Dynapath 30 will accept a negitive CC value. MasterCam produces flawless code for my Dynapaths!

[mmonica]

I forgot to add, I always use lead in/out values with cutter comp!

[M. Anderson]

Thanks guys, (gals' if present)

 

I do use both, lead/arc in and lead/arc out. The problem seems to still occur - it is like the control is reading the cutter comp " 2 (TWO)" lines ahead! In other words the cutter comp is posted to be turned off on the last linear part of the "lead out", but the control is still on the last part of the posted "contour/pocket" and turning off while still cutting!

 

OH! Call Dynapath - they just think I am crazy! But it is pretty straight forward - watch the control display line (CO-OFF), or measure the pocket wall, IT IS TURNING OFF!

 

Now the only way I have found around this is to enter/exit at a "point", and use both "lead/arc in" and "lead/arc out". That way there is a extra move from and to the enter/exit point! So far this is working! Till I have a contour/pocket with no room to do this in.

 

mmonica and Surface:

 

My Delta 20 control does seem to accept negative cutter dia. offsets! Running one today and had to move the cutter dia. down to -.0093, to get the pocket cut to correct dim. JUST LOVE RE-GRINDS!

 

You may want too recheck your control? Or NOT, if it works for you, leave it alone!!!!

 

Our control is on a ZPS-Tree VMC840, 1994-5 model machine. Problem maybe model, year specific? I don't know, but this control is not on my FAVORITE list, for sure!

 

Everybody: Thanks for your sugestions and help!

 

I guess I will have to go down to GA and see my dealer, I don't seem to have made them understand about the problems with the drilling cycles. If it shows the tool returning to a clearance height of 1" above the part in the backplot of the tool path, I very well expect the post to output the correct code for this to occur! NOT move between points at .05 above 0 (zero)! Since this is something you can turn on/off, mabey the post just is not set to handle this? And G98/99 is not the problem.

 

Thanks again,

 

Mark