Newbie here, with a question already....TIA.

[A3kid]

Does anybody here have any experience running a Thermwood 3 axis router w/ Mastercam generated g-code?

 

We just purchased a used one & had the contoller upgraded to the new 91000 Supercontrol, and I've got a few questions I could sure use some assistance with.

 

Thanks in advance.

[chris m]

There are a bunch of router guys here and I know that some have Thermwoods; you will probably need to wait 'til Monday for a big response, though.

 

May I suggest that you read the Forum Guidelines / FAQs in the mean time, if you haven't already; it'll keep you from getting bonked next week.

 

Welcome aboard

 

C

[A3kid]

Thanks C.

 

I read the guidelines. I'm not a newbie to discussion forums and the character hierarchy that exists in them.

 

I'm up to my butt in alligators right now with a project here at work - trying to machine molds for our vacuum form machine. I know I'll probably get beat up for asking for help so soon,

but I'll weather the storm when it comes.

 

At least I didn't ask for a post processor...

[crazy^millman]

We have a Model 67 5 axis Machine with the same controller. You can probaly use a standard fanuc code post for the machine and it will work fine. If you want soemthing custom then you will need to talk to your dealer or learn hwo to do your own post modifications. Here is a sample what my post outputs for me.

code:

---

(T6  | 1.5 FACE MILL            | H6  | M6  |  DIA. - 2."  | R0.3100 | FACING)

(T1 | 1/4 FLAT ENDMILL | H1 | M1 | DIA. - .25" | | CONTOUR)

 

 

[WINDOW OFF]

( Thermwood Model 67 5-Axis Router )

( Mastercam Version 9 - THERMWOOD )

( MC9 FILE - C:2004_MC9 THERMWOOD TABLE HOLES .MC9 )

( PROGRAM LOCATION - THERMDATAPART SPINDLE NC )

( DATE - 22-01-04 )

( TIME - 18:40 )

 

 

( Tool count: 2 )

 

( ************************************************** )

SET TLPOST =12.777

( ************************************************** )

 

G90 G70 G40

G96 G43

G990

M999

 

( Tangency Factor - 8 = Default )

G09 F20 (THIS IS USER SET ON THE MISC PAGE

AND ADJUTSABLE FOR EACH OPERATION)

( Acceleration Macro - G800 = Default )

G805 (Accleration Macro) (THIS IS USER SET ON THE MISC PAGE

AND ADJUSTABLE FOR EACH OPERATION)

[WINDOW ON]

[PRINT "T6 1.5 FACE MILL FACING"]

[PRINT "T1 1/4 FLAT ENDMILL CONTOUR"]

[PRINT "THESE ARE THE TOOL FOR THIS PROGRAM"]

[PRINT "MAKE SURE THEY ARE IN THE THE TOOLCHANGER"]

[PRINT "IF THEY ARE HIT THE GREEN BUTTON."]

M00

[WINDOW OFF]

[WINDOW ON]

( *** ENTER REFERENCE COORDINATES FOR Y TABLE BELOW *** )

( *** X = Negative, Y = Negative, Z = Positive *** )

SET X1 = 0

SET Y1 = 0

SET Z1 = 8.256

 

( ************* CONTROL SECTION ************* )

SET TX1 = X1

G92 X[TX1] Y[Y1] Z[Z1]

[WINDOW OFF]

[CLS] (THIS WHOLE SECTION IS USER INPUT IF THEY WANT OT SET

(THE Z VAULE IN THE MISC OR USE THE Z IN THE G52)

M98PSTRTTIME.SUBL1 (THIS CAN BE TURNED ON IN THE MISC)

M48 (THIS IS TURNED ON AND OFF FOR POSTING IN THE MISC)

(OVERALL MAX - Z.25 )

(OVERALL MIN - Z-.5 )

( ************* START PROGRAM CODE ************* )

( 1.5" FACE MILL TOOL - 6 DIA. OFF. - 6 PIVOT LEN. - 12.777 DIA. - 2. )

G70

T6

( MAX - Z.25 )

( MIN - Z0. )

S20000 M03

M31

G52 L1 (USES THIS FROM WORKOFFSETS)

G00 G90 X59.9999 Y-1.2 C0. B0.(MOVE TO ALL 4 PLACES AT ONCE)

G47 (APPLY HEIGHT OFFSETS TO THE NEXT MOVE)

G00 Z6. (USER DEFINED IN THE MISC ALLOW FOR DIFFERENT ONES IN 3 AXIS OR 5 AXIS)

Z.25

(BODY OF PROGRAM

G00 Z.25

G46

G00 Z6. (USER DEFINED IN THE MISC ALLOW FOR DIFFERENT ONES IN 3 AXIS OR 5 AXIS)

M01

G800

( 1/4 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 PIVOT LEN. - 12.777 DIA. - .25 )

T1

( MAX - Z.25 )

( MIN - Z-.5 )

S24000 M03

M31

G00 G90 X46.1113 Y14.9743 C0. B0.

G47

G00 Z6. (USER DEFINED IN THE MISC ALLOW FOR DIFFERENT ONES IN 3 AXIS OR 5 AXIS)

(BODY OF THE PROGRAM)

G00 Z.25

G46

G00 Z6. (USER DEFINED IN THE MISC ALLOW FOR DIFFERENT ONES IN 3 AXIS OR 5 AXIS)

M49 (THIS IS TURNED ON AND OFF FOR POSTING IN THE MISC)

( ************* END PROGRAM CODE ************* )

M98PENDTIME.SUB1 (THIS CAN BE TURNED ON IN THE MISC)

G43

G990

G94

G00 Z0

M05

G00 C0 B0 X0 Y0

M02

---

I was lucky to get soemthing close and then just did some modifications from there. I am having trouble getting it to work with 5 axis very well but I am not lucky in talking the owners into a $$$$$$$$$ post for our machine.

 

Good luck and I think you will enjoy the machien and the controller.

[A3kid]

Hey, thanks.

 

My question is so rudimentary I almost hate to ask it in public...

 

I've got a post processor that works, from my understanding that's the tough part.

 

I can't get the machine to recognize the darned "SET ZSHIFT=" command. I enter the daylight value in the tool setup (F9/F2) window, but no matter what I put in for the zshift value, the machine ignores it.

 

What the heck am I overlooking????? (Obviously, something I've forgotten from programming school..)

 

Thanks again, and sorry for the questions.

[chris m]

quote:

---

At least I didn't ask for a post processor...

---

That's what I was worried about when I saw the ' does anyone run this control with Mastercam code? ' question. I hate to see guys get torched right off the bat .

 

I know NOTHING about routers so I'm no help, just bump the topic on Monday morning and I'm sure you'll get some help if Ron can't help you.

 

C

[crazy^millman]

Ok well here is where the fun begins on a Thermwood. I dont use the set Z I use the G52. If you are going to use the set Z then you dont uise the day light for the tool.

 

If you are going to use the Daylight you need to set this up on the acutor page with number 2 aucator. If your machine is set up with 2 acuator postion but it may not be since you have a 3 axis machine. The best way I can explain daylight on a Thermwood is that your z vaule for Z 0 of the program is the daylight vaule for that tool and that tool only. If you use a set z and do not use the tooloffset then you only have a vaule good for one tool. That is why I use the tooloffset the G47 way with a clearence move after that call and then use the g52 as my postion location for x,y,z on my 5 axis machine. It works like a champ. The reason I dont use G45 is when you call it the machine move ot the tooloffset length and if you are in a tight space not good. So with the G47 and then your clearence move you know you are safe.

 

The G52 is the same as G53 the only different is the G53 moves the table upon call where as the G52 moves to the positon when you tell it to move the postion realtive to the G52 postion offset. I like full control over my moves and the G53 and the G45 take that away from you and give it to the machien that sucks and I recommend stayign away from that. I have made my post use the G52 via this code you are welcome to try it but ALWAYS MAKE A BACKUP COPY OF YOUR POST BEFORE DOING ANY MODIFICATIONS:

code:

---

pwcs            #G52+ coordinate setting at toolchange

if use_frst_wcs < two,

[

if workofs <> prv_workofs | (force_wcs & toolchng > zero),

[

p_wcs = workofs

"G52", *p_wcs

if mill_plus, result = mprint(swcserror)

]

!workofs

]

---

This should get you going we can talk about other things later for now if your post does not have the G47 just hand edit and we will work on that next.

 

Here is what I would do before and after each toolchange call.

code:

---

G47 

G00 Z6.

Then body of program

G46

Z6.0

---

I use 6" cause I have the room you may need soemthing less just remember this amount needs to always be more than the tool offset and you should be good.

[crazy^millman]

One other thing there is nothing easy about the supercontroller at first it is like no other machine but like every machine you just have to figure out its quirks once you get that down then it is all smooth sailing from there.

 

Do you have the auto toolchanger and did they show you how to open it from manunal. Did they show you how to normalize the axis. One other thing their book for tramming the head on a 5 axis lacks alot like pictures of where they are really talking about so I made my own in Word using Digital pictures so that if my operators need to fix the machine they can. They want you to go spend a week in their school for all this crap and sorry guy but I got better things to do with my time. Ask and I and otehrs will be glad ot assit you and Yes good move on your part ot not ask for the post that will win alot of respect among the community.

 

OH YEAH FORGOT TO SAY WELCOME TO THE FORUM

[A3kid]

Ron,

The machine is an OLD 3-axis unit w/o tool changers, 2 non-programmable spindles, and one drill head.

I'm well versed w/ the G52 & G53 fixture offsets, and have written a few programs that switch heads (G26ZW / G27) and use multiple fixture offsets. The problem is, the post I've got is specifically set up to use the "set zshift" command. It prompts for "Material thickness", "G92 x value", and "G92 y value" just prior to writing the posted code.

The darned thing is set up to use the only feature I can't seem to make work right on the controller! And I'm finding that rather aggrevating.

 

Deep breaths.

Calm blue ocean.

Calm blue ocean.

[crazy^millman]

Well the thing about the set vaules is that they are the oppsite of what you put in a G52 or G53. That is why I hate them.

 

Look for that section in your post and take it out.

 

Oh eyah one mroe thing you can not use the set with the G52 you have to use either or that is why I have mine as a misc in my post if I want them then I just put a z vuale in my Mr10 and if I dont want them I use the workoffsets.

[Thad]

quote:

---

Deep breaths.

Calm blue ocean.

Calm blue ocean.

---

I like that.

 

Welcome to the board, Scott.

 

Thad

[A3kid]

A shameless BTT, +1 & bump - hoping some of the Thermwood programmers will read this.

 

Thanks for the "Welcome Aboard", Thad.

 

[acerx3]

This is my first attempt at returning a tiny bit of the vast amount of help I have gotten from this forum over the last couple years so please bear with me.

I have 2 Thermwoods and use the "SET ZSHIFT=" on both of them. The daylight value is the distance from the tooling to the table top and the "ZSHIFT" value is 1)the thickness of the spoilboard or 2)spoilboard plus part thickness, depending on your Z zero in mcam. Operators change this value when the spoilboard changes.

HTH

I'm just a wood butcher and feel very humbled/intimidated by the amount of knowledge expressed by the real machinists in here.

 

I'll be glad to help if I can though.

[A3kid]

Thanks acerx3. We're just at the woodbutcher stage ourselves when comes to milling. I've run CNC lasers for about 9 years, but this IS a different game.

 

To those who answered and tried to help - after many conversations with the tech team at Thermwood, and getting "help" that didn't, I dug into the actuator setup menu and found that the machine hadn't been properly configured when they finished the controller upgrade. The support team didn't know that, and couldn't understand why none of the advice they were giving me didn't help. They were getting to the point of "What's the matter? Are ya stupid?"

 

I fixed a few of the major issues with actuator 1, and ran the most complex of the 11 sections I need to cut yesterday with only 2 minor changes to the posted code. It didn't come out exactly the way I wanted it to, but now that it's running I can watch it and learn what I need to change from there.

 

Thanks again, to all who attempted to help. I greatly appreciate it.

[crazy^millman]

Yeah that is where the Thermwood is different than any other machine. The different heads are your deal there. I have acuators changes for 3 to 5 axis so I also have to be careful they are right. Well I am glad you are going in the right direction good luck and hopefully we can be of more help in the future.