Post Processor B Axis Modification ..

[Anonymous]

Hello again .. I have a question to see if you can help me ..

Previously I made some queries for the modification of a post processor for a cnc with Syntec 6MD controller .. using the base of FANUC I managed to make it work ..

Now studying a little more in detail the code I see that there are things that are not well resolved ..

My CNC have rotation axis B, that is, it rotates on the Y axis, +90 -90 degrees ..

It has a tool length compensation system, but it does not have RTCP or TCP enabled .. and this is where I have the doubt ..

In the code that I generate, I can perform operations on 3 sides of the piece, making the tool rotate on them. upper, left and right .. but when performing the lateral perforations, the head uses the X axis as depth instead of Z, which leads me to that the height compensation of the tool vary the height of the lateral perforation of the piece ..

The initial doubt is .. the correct way is to make it in cnc when you perform an operation with the spindle rotated 90 degrees, take that the depth is X or Z?

%
O1002 (TEST 2)
(T5 D=6. CR=0. - FLAT END MILL)
G90 G94 G17 G49 G40 G80
G71
G53 G00 Z0.

(DRILL1)
T5 M06
(ATC TOOL 5)
( S20000 M03 )
G56
G00 B0.
G00 G43 X8. Y32. Z222.4 H05
G00 Z197.4
G98 G81 X8. Y32. Z192.39 R197.4 F800.
Y64.
Y96.
G80
Z222.4
(Move the spindle to avoid collision with the part.)
G53 G00 Z0.
G53 G00 B0.
G53 G00 X0.
G53 G00 Z0.

(DRILL2)
G00 B90.
G49
G00 G43 X-383.5 Y32. Z-145.3 H05
G00 X-333.5
G01 X-328.49 F800.
G00 X-333.5
Y64.
G01 X-328.49 F800.
G00 X-333.5
Y96.
G01 X-328.49 F800.
G00 X-333.5
X-383.5
(Move the spindle to avoid collision with the part.)
G53 G00 Z0.
G53 G00 B0.
G53 G00 X1600.
G53 G00 Z0.

(DRILL3)
G00 B-90.
G49
G00 G43 X694.5 Y32. Z-145.3 H05
G00 X644.5
G19 G81 X639.49 Y32. Z-145.3 R644.5 F800.
Y64.
Y96.
G80
X694.5 Z-145.3
G17

G53 G00 Z0.
G49
G00 B0.
(STOP SPINDLE)
M05
M30
%

As seen in the code, in red mark where the spindle rotates to its position .. and in G43 the tool length compensation is activated .. but since it takes it on the Z axis, what varies is the height of the tool. the perforation, not the depth ..

I appreciate what they can contribute ..

[seth.madore]

Two Three things:

1) Can you share your Fusion file that you are using to generate this code

2) Can you also share the Post Processor that you are using?

3) Can you hand write the code that you EXPECT to be seeing (not what is produced)?

[Anonymous]

Hello Seth how are you?

Yes of course I leave both files attached.

About what I'm getting from the final code ... it's part of what I'm trying to consult .. (I apologize because English is not my native language and it's often difficult for me to express myself through a translator)

How would it be the correct way? that the team when the spindle rotates at 90 degrees, change the planes and when the code moves the Z axis, instead of making the movement vertically, do it horizontally?

Or how do you currently rotate the spindle and move on the X axis?

Please tell me if it is not understood and I will try to write it in another way ..

Thank you !

[Anonymous]

Project file ..

[seth.madore]

Ohhh, that's right. You have the rotating head machine. 

It all comes down to what your machine needs to see for code. That is not something we can answer, but only you, others with your same machine, or the manufacturer of the machine. Look for programming examples and programming manuals that list the "DO" and "DO NOT"

What is your native language, if I may ask?

[Anonymous]

Thanks Seth .. yes of course .. my language is Spanish ..

On the issue of what the machine can or can not do ... well ... it has a rotary head on the Y axis .. as far as I could read, that rotation is called the B axis .. it turns +90 -90 degrees ..

The machine has ATC with a linear bench of 8 tools .. It has height sensor of the same and the capacity of height compensation of tools (G43) as seen in the code ..

What it does not have is TCP (or RTCP) .. so I have to perform those rotation calculations through the software or post processor ..

I have tried with examples and other processors .. but my cnc does not support commands such as G68.2 etc. if it supports the G68 but I do not know if that procedure is correct ..

Believe me if I go to write is because I have been trying to solve months through web information, sample processors etc ..

I have modified almost all the sample processors and similar manufacturers that are available by autodesk .. but I am confused at this point ..

I do not pretend to be solved ... but if you can help me or just guide me on the right path I would be more than satisfied ..

[seth.madore]

When you tip your machine head at 90+/- degrees, what happens when you move the spindle in what would normally be the X direction? Does the Z value change, or does it still continue posting it's location as if the spindle was still vertical? Do you have a programming or operation manual for this machine?

[Anonymous]

If I break the head of the machine, at any angle the movements of the machine do not vary .. the X, Y or Z axis continue to move in their normal position ..

Eg if I program a Z-axis movement from 200 to 100 mm .. it moves vertically .. if the head is broken 90 degrees .. it continues to move vertically ..

The only information about the machine that I have is that I found on the internet by Syntec .. but it really does not indicate anything about how to proceed with these movements .. and the controller that is a Syntec 6MD I chose at the time because it just has the ability to work with 5 axes ..

[seth.madore]

---

@Anonymous wrote:

I have tried with examples and other processors .. but my cnc does not support commands such as G68.2 etc. if it supports the G68 but I do not know if that procedure is correct ..

---

Looking at THIS MANUAL on page 87, it gives us the "how to" regarding coordinate rotation. Theoretically, you should be able to manually write a short program along their guidelines and execute a rotation. What happens to your machine then?

[Anonymous]

I've already tried that .. and it works but in fixed planes ..

G17 (X-Y), G18 (X-Z) and G19 (Y-Z) .. and then the parameter G68 enables a rotation in degrees on the selected plane, but not between planes as does the G68.2 in FANUC ..

For ex. if we wanted to make a hole in a face at 45 degrees this does not work ..

Anyway I'm trying to incorporate this to the post processor to at least solve the perforations in 3 sides of the piece .. the issue here is how to coordinate the movement of the axis that corresponds to the position of the tool to be able to use the compensation to through parameter G43 ..

At this moment I am seeing here how I should modify the post processor so that when the spindle rotates to +90 or -90 I will load in the code a G19 which would work in the YZ plane and transpose the movements of the cam to the corresponding axes ..

[Anonymous]

Hello again !

Well here I am refloating this topic in the forum .. I have not stopped programming and researching ..

I think I have found the key to my problem .. as I mentioned before, I have a 4 axis CNC .. X, Y, Z, B .. my big problem is that my controller does not support TCP .. and besides that does not have the advanced positioning options active .. as for example to use commands like G68.2 or G43.4 ..

Then I began to study other post processors such as "FANUC - Inverse Time and A-axis", "Thermwood 5-Axis", "5AXISMAKER" and others ..

In addition to this I often study the autodesk post processor manual for fusion.

But none of this covers my doubts .. I consult ... is it possible to control a cnc like mine by software through the post processor without having enabled the previously mentioned advanced options like G68.2 or G43.4?

If so ... because the information in the post processor manual differs so much from the post processors mentioned?

Let's say that I have achieved some results but none that really is worthy of calling it a solution!

I appreciate your help ..

[Anonymous]

Hi,

I have the same troubles.

I´m using the FANUC (with g91)/fanuc incremental on a machine with syntec 6mb

Must modify all my g-codes changing the g21 by g71 and deleting the duplicated "T" after a tool change, but I have no any other issues running any 3 axis milling operations/programs.

The troubles appears when I try to use the 4th axis.

Anyone find a solution for the g68.2 and g53.1 commands ?

Thanks

[manfred.raffler]

I have the problem that my B Axis is turning around Y as it should, but if I have a chamfer the position is not correct. I use Syntec controller 21MA. Maybe you solved this issue already. Thanks for reply

[CNCWoodarts]

same issue here, did you get this figured out?

[infoSDJP6]

Hi @Anonymous,

I have the same problem with IGOLDEN CNC machine. I have tried a lot of thing but I modified your postprocessor at line 397

var pivotDistance = toPreciseUnit(396, MM); // 311 + T3 // distance to pivot point along B-axis

where 396 is my pivot distance of 311mm with tool length of 85mm added. Wheh I run the program I delete the H03 tool compensation from G code and it runs right where needed.

Since I am not much into programming I will have to create a different postprocessor for every tool I have but I guess that pivotDistance can be set to 311 + tool length?

[manfred.raffler]

We are working in Autocad Fusion and we have a Syntec 21MA.

We solve it in this way inside the postprocessor:

headOffset = tool.overallLength + pivotDistance; // control will compensate for tool length

In Fusion 360 you have in the tool library the "overallLength" of each tool

[infoSDJP6]

Thanks,

I had that line but as a comment, it works like a charm now with tool.bodyLength