Posting to Thermwood 67

[xform precision creations]

I am just starting to post files to our Thermwood 67 machine that we have just installed. When posting it prompts for some fields. A couple of them I don't understand and was hoping someone with a similar machine can help me out.

It asks for 'Enter ref tool length'. What does this mean? I thought that it used the values that are set up through the tool library and therefore was already defined. Each tool would have a different ref length I would have thought?

Also it asks for 'rapid height for tool/op changes'. Is this the height it moves to to change tools (flip dual end spindle over) and is measured from machine home position.

Also don't really understand the part offset choices of G92 G51 G52 G53.

Thanks.

[Thad]

Ron, the Crazy Millman, should be chiming in any second now.

 

Thad

[Keithm]

I think that the ref tool length is a pivot length. The lenght from the spindle hard point the the end of the tool.

[crazy^millman]

Disclaimer my spelling and typing skills suck so sorry to offend anyone with that.

 

Sorry to chim in late here no internet at the house yet.

 

Rapid height is the distance from your part to the place to do the head movement and I beleive you have absolute and incremental control over this. The size fo the part and the limits of your machien have the biggest effect on this. I find that a reference point helps in thsoe tight places.

 

Ok let me see if I can give you some insight to the machine. The post I use and the post that you get from Thermwood allows you to do this in the post for that question.

code:

---

#Tool length, typically for head/head machine, both set to zero disables

#Applied to the tool length, RA applies this along the tool

use_tlength : 0 #Use tool length, read from tool overall length

#0=Use 'toollength' var, 1=Mastercam OAL, 2=Prompt

toollength : 12.813#Tool length if not read from overall length

shift_z_pvt : 1 #Shift Z by tool length, head/head program to pivot (Z axis only)

#0=Pivot, 1=Pivot-Z, 2=Tool Tip Programming (without zero length)

#Option 2, So we can still take advantage of brk_mv_head feature

---

I always use the tooleye and the tooloffset page to set up my tools and I never use the spoil board for 3 axis machining. This goes against the very idea that Thermwood has on how to use their machine but to me is the best way to use their machine. In using the machine this way you need to use the toollength calls which are G47 on for actavation on next move and G46 off for next move after call. I have hard coded my post to be at 4" but you can make this vaule anything you want. I do not use the G45 on and G44 off set up becuse you have no control where it is going and I feel this more a possiblity of a crash this way. The other thign if doing 5axis work write yourself a run in cycle to do in the morning and the eneveing for about 45 minutes on the 4th and 5th axis. Here is a sample of that program:

code:

---

T1

M98PSTRTTIME.SUBL1

M80L5

G00 G90 X30.

G01 C360. B135. F200.

G04 F15.

G01 C0. B-135.

G04 F15.

G01 C360. B135.

G04 F15.

G01 C0. B-135.

G04 F15.

M83

M82L5(COPY THIS AS MANY TIMES AS YOU WANT)

M82L5

M98PENDTIME.SUBL1

---

I also check the tramming about once a week by running the 4th axis 360 with an indicator. I also made my own tram bar and saved big bucks and got soemthign that is 100 times better than a bent piece of steel.

 

Now here comes the most intresting part of the Thermwood and that is the workoffsets and what is the best way. I do not use the set x,y,z method that the post they problay gave you does and I do not use the G92 method that this uses either. I do not use the G53 workoffset becuase they also take the control away fro myou on where the machine is going to go. If you use the G53 the machine moves ot that place whne G53 and the postion is called where as with the G52 method you to me get a flow of the program and the machine all at your control. I use the G52 LXX for my offsets and use the workoffset from the toolpage. THe cool thing is that 1=G52 L1 and 2=G52 L2 and so forth. Here is that section out of my post:

code:

---

pwcs            #G54+ 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

]

---

I use an edge finder find where I want put that in my corresponding postion in the workoffset page and go from there. I also use the Z vaule for zero vaule for the part. The tooleye and the post do all the rest of the work for you. This again is my method and from what I understand goes against conventional wisdom for Thermwood but kicks some serious but as far as I am concerned. The only other thing I can tell you is get fimaliar with your tangancey codes and also with your M48 and M49 rapid feedrate override. I have this and the timer as Misc in my post so that I can actavate them when I want. I also have my post set-up where if I am usig nthe M48 then I turns off the override for toolchanges and then turns it back on for machining parts save a good bit of time on a 10' table. I think the biggest thing that is the probelm is the screwy book which a bunch of double talk.

 

I think the biggest thing I can also tel lyou is watch your Misc for 5 axis machining the MP5XGEN will crash your machine even with all the correct Misc vaules used. I have added alot of things to my post to keep this from happening but still do not trust things 100% at this point and with no verfication software I have redunt stuff in my post but I know it is safe to run for 60 hopurs and not have a crash. Good luck and I hope that lengthy explaintion helps if you need mroe information please ask more than willing to help.

 

This information is my personal opinion and is given to help not hinder in anyway. If you use this information in anyway do so at your own caution. Thank you and have a nice day.

[MATT Q]

When I use the rapid heighth in the post is I set my home position at the highest z plane on the part and then use a postive number and the machine will retract that number above the home position and reposition to the next toolpath operation. The reference tool length I use is what they describe in the book by touching off the tool on an indicator straight up and down and then flipping axis 5 90 degrees and moving the machine down in the z and touching the shaft off on the indicator and then moving down the radius of the pin to be in the center of the shaft. You take those two z values subtract them and their is your reference tool length. Unless you have a tool eye and it does it for you like Ron said.

 

Oh yea learn how to TRAM you will need to know how to do this to be accurate and do it often especially after a crash if that happens.

[crazy^millman]

No Matt you are correct about the povit distance figuring or tool length offset as they call it. The tooleye is so that once you have this distance you only need to touch off the tools and go from there with the post and Mastercam is what I meant to explain.

 

 

This information is my personal opinion and is given to help not hinder in anyway. If you use this information in anyway do so at your own caution. Thank you and have a nice day.

[xform precision creations]

Thankyou for all the infomation. I will enter some values and experiment with different settings and see how I go.