Thermwood Insight (i.e. Help)

[Slick]

So I currently metal applications where I work. And have brought MasterCAM into the company's 5-axis realm as well. I now am looking into getting things rolling in their 3-Axis world. I have taken a Generic Fanuc post and edited it to make code with, and my first test run worked no problem. Now I am embarking on an actual production part and wala! The code is wierding out on me. For some reason in the graphic display it is showing the machine wants to do some really funky arc moves, (backwards, i.e. the long way around). So I'm here asking if anybody has any advice, or maybe even a post for a Thermwood Model 53.

[gstephens]

I STRONGLY suggest contacting your Mastercam dealer or Thermwood directly (thay can get you a post). The Thermwood controls are notorious for being different between different machine serial numbers.

 

That being said, It sounds to me like your control is placed on the weird side of the machine. Make sure that the "right-hand-rule" is in effect for your machine. you may have to reverse the "G2" and "G3" outputs as well as change direction of incremental arc centers (especially in XZ,ZY planes).

[Zero]

You can try setting you filter to have a larger minimum arc radius, or look for the arccheck in your post (if it has one). Make sure it is set to : 1 and the ltol is something significant like .1. This will have your post find arc moves with a length smaller then the tolerence you input and convert them to linear moves. I had this same problem a while back and thats what fixed it for me. You also want to make sure you have the latest appmch patch for MC.

 

If problems still persist, you should probably contact your dealer.

[Ron Roderick]

Slick,

Have you tried combining your views before applying your toolpaths.

Ron

[Slick]

Ron, I guess I don't understand the question: "Combining my views". Feel free to explain.

I'm thinking gstephens is on to a similar thing that I am suspecting. We currently run another software to nest with, and it spits out a bunch of macros in a subroutine format. I ran a program on graphics that was ran correctly a week a go and now it's showing on graphics incorrectly, so I'm thinking this other software is swithcing something on "modally", that I haven't quite figured out yet. I'm calling Thermwood today about it. If anybody else is curious to the answer I come up with let me know, and I'll let you know what they say. Thanks for the help!

[Ron Roderick]

Slick,

When I bring in a File usually from ug usually as a parasolid , I go to the main menu, screen, next, and combine views. It changes all arcs to the same view. Some toolpaths such as wire frame 2d swept, will give all kinds of weird toolpaths if we don't combine our views.

Ron

[Slick]

I think I have ironed it out, but haven't proven it yet. Thermwood sent me an example post, and in comparing it with the one I have edited, there's one noticeable difference. In a line of my code using G03's, and G02's, in some lines it only has one I, or J value i.e. G03 X14.75 Y19. J-.75, opposed to the Thermwood post which has G3 X14.75 Y19. I0. J-.75. Now I just have to figure out how to edit my post to put those "zero" values in it. Any insight???

[Guest]

Look for a block similar to this (this block came out of mpfan):

 

parc #Select the arc output

if arcoutput = zero | full_arc_flg | arc_pitch,

[

#Arc output for IJK

# If you do NOT want to force out the I,J,K values,

# remove the "*" asterisks on the *i, *j, *k 's below...

if plane = zero, *i, *j, k #XY plane code - G17

if plane = one , i, *j, *k #YZ plane code - G19

if plane = two , *i, j, *k #XZ plane code - G18

]

 

Make sure you have the asterisks next to the values you want forced out. Hope this helps.

[PE @ IHS]

Leaving I or J out of an arc command has the same effect as inputting I0 or J0.

 

I, J, and K are incremental arc vectors specifying the center of the arc from the start of the arc (as you all know). Therefore, inputting I0 is the same as not putting an I value at all. Your problem is probably something control specific as GSTEPHENS has suggested.

 

Peter Eigler

[Ray Sander from Battelle]

MasterCam has a post for the Model 67 5-axis machine (I know I helped them write it). I do not know if that will work for the Model 53 or not. Give them a call or email me if you want to try it.

[Pierre Côté]

gstephens: "The Thermwood controls are notorious for being different between different machine serial numbers."

 

- Actually it is more a question of production date and control model. Earlier machines used an inverted right-hand rule or a left hand rule for axis designations. Since the 9100 (or at least the 91000 Supercontrol) the default axis designations have been standardized to right-hand rule.

 

Peter E: "I, J, and K are incremental arc vectors specifying the center of the arc from the start of the arc (as you all know). Therefore, inputting I0 is the same as not putting an I value at all."

 

- The Thermwood control utilizes the I/J, I/K, or J/K arc center combinations to determine the intended plane. G17, G18 and G19 are not needed using this format.

 

AV8TOR: "MasterCam has a post for the Model 67 5-axis machine (I know I helped them write it). I do not know if that will work for the Model 53 or not. Give them a call or email me if you want to try it."

 

- Since a 5 axis post usually works with 5 axis tool length compensation and not with 3axis daylight values, and that C and A/B axis references may cause problems, it would probably be better to go with a 3 axis post. (PS Your email is not listed in your profile.)

 

Slick-

 

With regards to your Model 53:

1. Approx. age of the machine?

2. What model of Thermwood control?

3. What control software version?

4. Toolchanger (manual quick change, bar-style, typewriter or carosel), turret head or fixed tooling?

5. Equipped with conventional or universal vacuum, roller-holddown, auto load/unload?

 

Also:

What Mastercam product (Mill or Router) and version are you currently running with? (I assume Level 3/Pro since you work with 5 axis.)

 

Get back to me and we may be able to help you out with a post.

 

Pierre Cote

CNC Automation

[James Barnes]

I have a therwood model 53 post if you need it.

[Slick]

Pierre, thanks for your time in helping, I am currently pulled off of the "Thermwood 3-Axis" project here, and will probably be getting back to it later in the week. I will try to get the above information. As for now my simple solution was to "Convert Arcs" into splines, which I personally don't like as far as drive a cutter (Can you say machine gun rat tat tat tat!). But oh well, it has proven to be the quick fix! Thanks for all of your guts' help, and feel free to be looking for this topic to re-surface in the next couple of weeks.

[Slick]

Hey James, thanks for the offer, I'd love to try your post and see if it works! Drop me a line!