5 axis head/head homemade CNC - gcode generator

Hello, I'm from Brazil and new here. Not sure if I'm posting in the right place but I need help on the issue below. Please…

For the last 6 months I've been trying to generate gcode for my 5 axis CNC (head/head B&C axis on the head) and I couldn't do it. It became a nightmare!

About the machine: Mach3 with 6 axis screen plugin (Axis: X, Y, Z, B and C). B&C on the head.
I’ve tried already: Solidcam, Sprutcam and for the last MasterCam 2017. In every one I wasn’t able to create the gcode for some reason (post processor, feature not available, complex difficulties, etc). My goal is to cut 3d surface in foam for molding - thing that I do with pretty easy with Cambam in 3 axis machine.

In my last try I had a modified (did my self) - Generic Fanuc 5X Router 1.pst – that could work with mach3. I tried this post processor with Mastercam, but this program it’s so hard to use that I had to quit – looking in the www, I’m not the only one who ran from it.

I have some experience: I’ve been using CamBam for more than 5 years for 3 axis and another program for 4 axis. Also, I have a small lathe that I create my own gcodes with the Excel.

Does anyone, please, can give me a hint were to go next?

To manage Head/Head CNC the RTCP feature is a MUST !
Table/Table configurations can, in same way, generate 5 axis toolpath without RTCP but with a lot of limits:

- overall speed
- precision
- gcode dimension
- kinematics of table must be very very simple with all pivots (H & J) set to mechanical 0 (zero).
- in cad placement of zero must be the same of machine table.
- feed control is not on TCP but in jonts so feed is inconsistent
- etc.

For HEAD/HEAD is yet more complex because you have to define perfectly the tool-length and add
all info of kinematics (rule, math, etc) in the post-processor.

With RTCP this is not necessary because is CNC to "accomodate" all in run-time.

Mach3 does not support RTCP in anyway so to do a true working CNC you have to choice another control board
with RTCP feature.

Many thanks for your quick reply! :)

Well, you gave me a lot of information that I was not aware of it. Let me unsderstand about RTCP at first and then I'll go back to my problem.

Thanks again,

Marcos

I know nothing about Mach 3 and while I am extremely interested in 5 axis machining,until I can find a legal 5 axis CAM system at a modest price I won't be going there.I do know that LinuxCNC can cope with up to 9 axes and it costs nothing;you can read a little about it here https://forum.linuxcnc.org/38-genera...-a-5-axis-mill.

I don't understand the description of the way the axes work in the OP and on this page there are several varieties of 5 axis systems https://www.shentuautomation.com/nrw...real-five-axis .It would be useful to know which is being described.I would be fascinated to know what form of 5 axis machining is being contemplated as a home built machine with the ability to use a home generated 5 axis continuous movement routine is the holy grail.Even a machine with the B and C axis fixed and using the other three axes to cut sections of a complex object would be a fantastic thing to have.

Do you have a tool setter to ensure that all tool tips are set at the same distance from the pivot or is there a tool length sensor that requires the controller to apply a modification factor?

Well, I thought it would be easy to generate 5 axis head/head gcode. There is a guy in Korea doing exactly what I need with a homemade 5X CNC (https://www.youtube.com/watch?v=QrjT...channel=ArrayZ) . But he does not give any reply about what he is using. So, I’m still finding out what I need to make it work. I don't need high precision or worry about collision control - I'll be cutting foam close to the shape that I want. Thanks for the links and reply.

If I understand your problem correctly you need a transformation of TCP-coordinates into coordinates of machine axes.
That is a problem that can not be resolved by modifying your post processor. What you need is a dedicated software in your control which performs the necessary transformation in real time for each and every point on your contour.
Within a post processor the only possibility would be to generate a lot of very short NC-blocks in order to make sure that the contour error between two endpoints becomes negligible when interpolating the machine axes.
You will not feel happy with this kind of solution.

To resolve the kinematics for a table/table in CAM post-processor engine is not impossible, Fusion, Cimatron, etc, at example, does that.
The resulting toolpath is poor, obviously, feed on TCP can be calculated only for block to block (line) and this is not a good thing.
Also the piece placement is forced to be at one unique position, the 0/0/0 machine, where pivots for A/C or B/C should be placed either on 0/0/0 machine.
Any other change to machine zero placement complicate a lot the kinematics math made ad CAM/Post level.

Resolve a kinematics for Head/Head in CAM post-processor is a hell because enter in calc also the tool-length (ignored in a table/table).

The only solution is to have a CAM that generates RTCP movements (eg: G43.4 for fanuc world) and leave to CNC board make the run-time kinematics translations
from RTCP g-code positions to CNC machine joints axes.

I'm in the software develop group of an Italian CNC Board which support RTCP fanuc like g-code.
In my case we support Table/Table A/C or B/C and Tilting-Head (Head/Head) A/C (not B/C).

To create a good G-Code there are a lot of good CAD/CAM, I'm used with BobCAD/CAM which is a very good tool for 5 axis tool-path.
To work in 5 axis continous machining with Linux is a challenge, a true challenge, trust me.
I've take a look to kinematics module and it's lack of many many things, and startup it's not for the faint of heart :)
It is neccessary to have some skills in programming and place hands in kinematics code to solve some big issues inner.
I guess it is the result of an academic study but to become a true working module must be handled yet.

Kinematics math is not the only question.
Also a good look-ahead toolpath feed planner is required and very important on 5 axis machining.

Have you posted a question on the Korean guy's youtube page to ask what software he uses to generate the code?I suspect it isn't a home brewed solution and he might have inserted the relevant figures for his particular machine into an existing package.

I am a bit puzzled by the comments in post#7.I have run 5 axis machines under OS/2 and Windows,but not yet Linux and I don't think the operating system controlling the machine would make a significant difference.I can understand that generating the Gcode is very challenging as there isn't a functioning Linux CAM package that I know of.That may change in the future.I also find it interesting to see BobCad recommended for 5Axis work as I have often seen it described as an entry level package for 3 axis work and with annoying salesmen who pester anybody who shows any interest.

Hello to all, many thanks for everyone. :)

Well I’ve been working on that for the last 2 weeks on my spare time.

What I did so far:

1 – I was able to modify the 5x Fanuc gcode using this information - https://youtu.be/G591hDY-_O4
2 – Created a simple Gcode for that that 5x Fanuc pst inside the MCam (by the way – awesome program –but it is not easy). Simulated my machine inside of MC (very nice).
3 – Manually modified the gcode with problems running in Mach3 (It’s my first contact with Gcodes modifications).
4 – Ran the gcode in my machine.

Problem: The C and B movement are very choppy!

Now, I start to understand what you guys are talking about here. :)

So, because of this choppy movement you need to generate RTCP movements. Correct?

Thank you guys very much!

Marcos

If the movements are very choppy is there a way to adjust the acceleration factors of the machine?There might be a piece of code in the program header or the controller itself may have a parameter you can adjust.

Thank you. Well, the machine runs smooth, I believe it´s something else. There is part in the pst file that beaks large rotary moves. I created a big arc and made de gcode for it and this is when the choppy appears. Could be that too. I´ll try to change this parameters and see what happens. I know nothing about it… Do you? Many thanks.

Pst file:
brk_tol : .001 #Break up chordal tolerance for 'brk_mv_head'
brk_tol_m : .025 #Break up chordal tolerance for 'brk_mv_head', metric

I'm no expert,but would say that you have posted the lines relating to chordal deviation;the first seems to be Imperial and the second metric.What I certainly don't know is if this deviation is applied at the tool after calculating the distance to the 4th and 5th axes or if it just related to X and Y.

Movements are "choppy" because without RTCP you lose a lot of precision in movements between two g-code blocks (lines).
Internally a CNC with RTCP applyes the kinematics arms in every point which is difference in axis movement between two lines.

A) G01 X10 Y0 A10 B30 F1000
B) G01 X11 A12 B31

Between two lines with RTCP you have an impressive ammount of micro-positions to keep in kinematics
Without kinematics you just have a normal interpolation (linear) between two lines.

To make line A to line B you can take for eg: 100ms.
With a CNC which plans movements every ms you have 100 times the kinematics rules applyied to get run-time toolpath positions.
With a CNC without RTCP the kinematics arms are applied at CAM with Line cadence and not maximum CNC toolpath look-ahead planning system (usually bettwen 1..4ms).