Dynapath Delta 20

[M. Anderson]

Is anyone here running a Dynapath Delta 20 control on a VMC? I have a ZPS, Tree VMC840.

 

I am having some post problems with V8.1, and would like to at least see some code for this control cutting a inside pocket with cutter comp on in the control. This is a used machine we just got, and the post included in MC does not work correctly -even after some changes - or I may be setting the parameters in MC incorrectly? Don't really know which it is!

 

But if I could see the output of a post that does work cutting inside pockets, using the cutter comp in the control, I could most likely mod the post I have. Dynapath's manual is lacking in detail for correct code output structure and the standard MC post sure don't work.

 

Now running the CC in the computer works fine. It's just a pain changing the cutter dia as it wears!

 

Thanks, Mark

[jenks]

I have used the DELTA 20 since 1985, and used MASTERCAM for programming since 1993 (ESPIRIT before that, but that is a time of my life I want to forget). I have never had any luck getting cutter comp to work when posted from MASTERCAM. If I want to use cutter comp I must edit the program inserting the commands as needed. I'm also using th post that generates code in the conversational format.

 

On the other hand, the HAAS (VMC)post, and the OKUMA (LATHE)post work exactly as advertised.

[smirob]

Cutter Comp in Control is ingnored in many posts for the Pocket cutting toolpaths in MasterCAM.

Many times what I will do, is cut the part, get some measurments, then go back to MasterCAM and adjust my tool size to reflect the needed amount.

For example if I measure the pocket to be .002" too small, I will adjust my 1.0" cutter in my tool table to be .998". Its a little more cumbersome but effective for me. :})

[Marty A]

if i'm reading your resposne correctly smirob,what i do is use a pocket program to rough out a pocket, then a fin. bottom program, then i will use a contour program with cutter comp which is in my version. i'm using mill 8.1.1. i have only been programing for 3 months so i'm sure there's other and better way's.

[M. Anderson]

While, I am not a MC programming expert by far, I think using cutter comp in both the control and the computer will be the best for me, on this machine at least. It allows me too program a certain cutter size, but allows the operator to adjust the size of the cut as the cutter wears. Found that answer here, last night.

 

I am NOT going to rewrite the program every time I need to make a cutter size change - that is a joke - and would keep me busy all day re-posting programs for the guys running this machine. I don't do this for the other machines, but the posts are correct!

 

What I am looking for is someone who has some old programs wrote for a DELTA 20 control, or even better - a listing of the commands and formats for the control. The manuals I have don't go into great detail on the proper formating of the programs.

 

IE: what switches and controls are used in this control for what commands -EX: G3 = Peck drill in conversational format - but what switches are avaliable to controll it - W - Q - J. What commands cannot go on the same line, where does the control expect cutter comp to start - or end? Does it need a feed command on CC?

 

That info is not listed in the manual, and that is what I need to know for programming (proof reading) and modifying the post. The current posts avaliable don't control CC correctly in this control. What else does the post not control?

 

Currently - when posted with CC added in control - and is output in the program - machine makes big jumps or bumps as CC is added or ended. When you start or make a pass in a pocket and start your lead in or lead out move - cutter comp is added/canceled on the first/last linear move - but if you are starting in a hole or still setting against the pocket wall. Well, that just don't work so well with this controll as it makes a rapid jump to the center of the cutter BEFORE moving on the lead in/out.

 

Now that is scarry as #$@#! Try that with a 5/8's endmill! Scrap part - broke EM - and a bathroom break!

 

Thanks for your help - Mark

[HEAVY METAL]

HI, MA

I HAVE PUT A POST ON THE FTP SITE "DELTA 30" IN THE POST FOLDER, THAT I HAVE TWEAKED FOR OUR DYNAPATH 30.IT SHOULD BE PRETTY SIMILIAR GIVE IT A TRY, LET ME KNOW.WE SET ALL COMPS OFFSETS TO ZERO IN CONTROL AND USE COMP IN COMPUTER. THIS SHOULD ELIMATE THOSE BOG OFFSET JUMPS

[Rick Damiani]

quote:

---

Currently - when posted with CC added in control - and is output in the program - machine makes big jumps or bumps as CC is added or ended.

---

If I am reading this right, it sounds like CC is added all at once, at the rapid rate, at the start of the lead-in move rather than being added gradually over the length of the first linear feed move, and you have cutter comp in the computer set to 'off'. Is that right?

 

What you could try doing is turning on cutter comp in the control and in the computer. Then the comp values you enter in the control are the far smaller wear/undersize values rather than the full cutter radius (i.e. you'd enter -.0015 for a nominal .625 mill with an actual diameter of .622). You could then make your start holes oversized enough to allow for that move, and the move should be small enough that the machene won't bump too badly. Any pass that allows for a lead-in /lead-out move should start the cutter far enough away that the comp move won't be a problem.

 

[ 02-23-2003, 03:05 AM: Message edited by: Rick Damiani ]

[M. Anderson]

Heavy - Thanks for the post, I will give it a try!

Has to be better than what I currently have, if you are using it now to run a machine.

 

Rick - I came too that same conclusion from reading some of the postings here about cutter comp. and MC. You can also put in a feed control command after the cutter offset command and eliminate the jumping. Done tried this and it seems to work.

 

I cannot beleive that some people here don't use CC in the control! Running the offset in the computer alone would be fine if I had nothing else to do all day. I am not willing to rewrite a program just to make a offset to the cutters. I " ABSOLUTELY REFUSE " too not be able to control the cutter offsets in the control. I don't understand why anyone would be willing to operate a machine and not make cutter changes in the control. What do you do if you are using 10 - 16 different tools to make the part? Write a program for each tool? Re-wirte the program 100 times a day? If the post in MC don't output code that the control can use - then change the post. That is why I am looking for some specific info on this control. The control manuals that came with the machine suck!

 

Thanks for everyone's help!

 

Mark

[Rick Damiani]

quote:

---

I cannot beleive that some people here don't use CC in the control! [Frown] Running the offset in the computer alone would be fine if I had nothing else to do all day. I am not willing to rewrite a program just to make a offset to the cutters.

---

Nor should you have to. What I reccomend to my students is that you use wear compinsation rather than compinsate entirely in the computer or entirely in the control. In v8.1, your comp options are:

 

Wear Compinsation (reccomended)

-----------------

Computer: Left or Right

Control: Left or Right

Result: Program 'nominal' size cutters in MasterCAM, then enter cutter size difference in control's tool radius offset. Gives you better control over compinsaiton and allows you to preview it in MasterCAM, while still allowing the operator to adjust the offset to compinsate for wear and allows the use of re-ground cutters.

 

Computer Only (default)

-------------

Computer: Left or Right

Control: Off

Result: Must reprogram to use a re-ground cutter or to adjust for tool wear. Not reccomended for most situations.

 

Control Only (not generally reccomended)

------------

Computer: Off

Control: Left or Right

Result: Can use any cutter, within reason. May result in alarms in the control, as you won't be able to verify sucussful cutter comp until you know what tool has been selected. You have to use relativly long lead-in moves to allow for full radius moves at the control.

 

No Compinsation (not generally reccomended)

---------------

Computer: Off

Control: Off

Result: Everything is under/oversize by the cutter radius. Generally only used for engraving, pocket roughing, and surface toolpaths.

[M. Anderson]

HEAVY,

 

Thanks for the post processor file!!!!

 

It works much better than anything else I have found!

 

Thanks, Mark

[HEAVY METAL]

Hi Mark

Try using the edit jump[ routine this should out put a Z value with G0 then repeat drill cycle for next hole.Let me know if you have any other problems that need worked out I'll take a look see if I can help. I had to edit the post for the edit jump routine to work right.

[jspangler]

Hi

This is an old post, but since you are obviously able to get your programs into your Dynapath contraol, would you mind telling me your settings on your contorl and PC?

 

I can't get my PC to talk to my control ( Delta DYnapath 20 on a tree VMC 840).

 

Thanks

 

John

[bobknob]

HI, MA

I HAVE PUT A POST ON THE FTP SITE "DELTA 30" IN THE POST FOLDER, THAT I HAVE TWEAKED FOR OUR DYNAPATH 30.IT SHOULD BE PRETTY SIMILIAR GIVE IT A TRY, LET ME KNOW.WE SET ALL COMPS OFFSETS TO ZERO IN CONTROL AND USE COMP IN COMPUTER. THIS SHOULD ELIMATE THOSE BOG OFFSET JUMPS

hello sorry im new what ftp is that delta 30 sample post on i would like to compare it mine and clear up some issues

thank you in advance

[Müřlıń®]

What you do is to leave off cc for pocket and add a contour at the end with cc.