Biesse Machine and MeshCam - HELP

[nem3]

I am trying to use Meshcam to help us get more creative with routing. The problem I am having is that I cannot figure out how to reverse Meshcams Z depth numbers. Our machine uses vacuum pods to hold parts down. The top of the pod is Z0 everything above the pod (Where you route the material) is Z Negative. The higher you go the lower the number. So if you put a 1 inch thick board on the pod. The top of the board would be Z-25.40.

Everything below the pods is Z Positive. So when we want to route all the way through some the Z Depth would be something like Z6.00.

We actually use a different variable that is part of Biesse Cam software. But you guys get the idea.

When I run an STL through Meshcam, all the changes I made to the post work great and I am able to get the machine to run the program. The problem is that its basically cutting the opposite of what the STL was. Because all of the Z coordinates are figured the opposite of the way the machine runs.

The only way I can think of getting it to work properly is to just draw the part as a negative, so it routes out a positive. But that just seems to stupid for me to have to do.

Also the way the "other variable" works is from the top of the material down. So you set the material thickness in the program editor to let's say 20mm. And you want to route half way through the board. You would set "PRF=10.00". Which would actually be routing and Z-10.00 when your watching the console. Could I possible change the Z character to "PRF="

Any help is greatly appreciated. Thanks.

[kong]

A method that springs to mind is to open the g-code file in notepad and use edit->replace to change the z's to PRF=.

Also, I will move this thread to the Meshcam section where you may get some more help!

[nem3]

Thanks Kong, and sorry about that.

The only thing about changing them to PRF's is that I think I would need to put in the feed rates, plunge rates, spindle speed and tool correction at every line then. Because the way we run the machine for 2D parts is just set the PRF at the first line of geometry and its all X and Y from there on out.

It may work that way, and it something that I have not tried yet. But I would prefer to use the Z coordinates instead.

[anoel]

You can open the Gcode in Notepad and do a "Find and Replace" change "Z-" to something arbitrary like "QT" and then do a "Find replace" and change "Z" to "Z-" then turn around and do the "Find and Replace" again, changing "QT" to "Z"

That would reverse the Z like you are wanting to do.

I've done this on a number of occasions on my X axis to get mirror image parts.

[tauscnc]

1

[nem3]

Your not understanding the problem. Our machine works from the bottom of the material up. Meshcam works from the top of the material down. Changing the Z's in notepad will only give me a negative of what was originally modeled. I need to be able to change MCam to work from the bottom of the material up going from Z0.00 to Z-25.40 (for a one inch peice).

I thought that I could do this in the Translate Geometry menu. But it doesn't do anything to the Z's

[robgrz]

I can probably modify one of the existing post processor configs to generate code for your machine directly. I'm travelling right now so I won't probably have time to get to it for a few days. If you have a PDF file for your controller that you can point me to it would help.

Thanks,
Robert

[nem3]

That would be great Robert. I will post what the control codes are when I get home and a sample program of a 2D Route so you can get an idea of what the Biesse specific codes are.

Thanks, Nick

[tauscnc]

Hey nem3,

Good to see you here. Robert should be able to do the job considering he made MeshCAM...by the way Robert, I cut my first 3D part using it and it was "a piece of cake!" Thanks for an awesome program.

taus

[nem3]

N20 PAN=1 ST1="R9.5D" L=PCUA
N30 G46 X453.90 Y211.97 G41 F8.00 S18000 VF=2.00 TP1 PRF=26.00 L=PON M55
N40 G3 X462.84 Y203.03 I462.84 J211.97
N50 G1 X657.05 Y203.03
N60 G1 X657.05 Y3.00
N70 G1 X3.00 Y3.00
N80 G1 X3.00 Y422.10
N90 G1 X657.05 Y422.10
N100 G1 X657.05 Y222.08
N110 G1 X462.84 Y222.08
N120 G3 X453.90 Y213.14 I462.84 J213.14 G40
N130 G0 L=POFF
%


A little preface before I write the codes from the book. Our machine must use the N numbers, that I fixed in one of the posts. Also the coordinates must have spaces between them, or the machine throws an error.

G0 = Rapid Positioning move independent of programmed axis speed.

G1 = Linear interpolation move with a programmed speed.

G2 = Counter-clockwise circular interpolation move with a programmed speed and given center coordinates.

G3 = Clockwise circular interpolation move with a programmed speed and given center coordinates.

G4 = Counter-clockwise circular interpolation move with a programmed speed and given radius.

G5 = Clockwise circular interpolation move with a programmed speed and given radius.

G6 = Circular interpolation move with a programmed speed and tangent to previous movement.

G7 = Counter-clockwise elliptical interpolation move with a programmed speed and given semi-axis center coordinates.

G8 = Clockwise elliptical interpolation move with a programmed speed and given semi-axis center coordinates.

G40 = Cancellation of tool radius correction as shown. Center tool correction.

G41 = Applies tool radius correction as shown. Tool right of material moving up.

G42 = Applies tool radius correction as shown. Tool left of material moving up.

L=PCUA = Performs and automatic tool change.

L=POFF = Lifts router to Z park and turns is off.

L=PON = Turns router on and lowers it to the programmed PRF value.

L=PSU Positions the routing tool (with router remaining turned on) above the panels surface, to allow for a rapid positiioning move to the subsequent start point.

F = Assigns the machining feed speed to router, listed in meter/min. (Fastest speed we have used so far has been 16).

I = Defines the X axis coord of a center point.

J = Defines the Y axis coord of a center point.

K = Defines the Z axis coord of a center point.

M = Defines a machine instruction which is sent to the PLC (M55 is supposed to close the cover of the automatic tool change storage area) The problem is that there is no cover to close. So I don't understand why the PC based software puts this code in the GCode.

PAN = Identifies the number of a milling unit.

PRF = Lists the depth of machining.

S = Defines the rotation speed of the milling unit. If left blank, the assigned tool's rotational speed as listed in the Tool Table will be used.

TP = Identifies the number of the milling unit.

VF = Defines the vertical feed rate of a spindle.



The above was taken directly out of one of the books that came with the machine. I can not find anywhere what the G46 is for. But they also did not write the section for Cutter Compensation, Lead-ins and Lead-outs. The header page for that sections actually says "YET TO COME"

Also forgot to mention. I tried changing all the Z coord's to PRF's. The code ran, the only problem is that the PRF's need to be followed by something to reset the cutter depth. Either by a L=POFF or L=PSU. I did not have time to figure it out. But as you see PRF is only at the beginning of the program geometry.

The way I Think it works is that the PRF is set at the beginning of the geometry and the only thing that resets it is L=POFF or L=PSU. Because with both of those the router retracts to its home position.



For now that's all. If you need anything else or have any questions feel free to ask. And I will try to help.

I really appreciate your help on this. Thanks.

Nick

[MarkT]

The primary issue is that Biesse code in an Rt480 or XNC (NC1000) control is signifigantly different than standard EIA/ISO code. It relies on unique PLC programming and internal assisted subprograms. The code environment itself is NOT industry standard, rather Biesse standard. That said MeshCam should still be able to configure a post for it. I would be curious as to how it turned out?
Mark T.

[nem3]

Well I have yet to hear from Meshcam on how the post is going. On a further note. We have recently purchased Mastercam X2 as they finally have a post for the Biesse machines. All I can say is that they did an awesome job on the post. The Gcode looks exactly like it did from Biesse's software. Which is not what I had expected. There are still a few things we are tweaking, like our drill blocks. But other than that its great. Meshcam would still be very nice to have. As we have only purchased the Router 1 package, and cannot do any surfacing.