4 axis cnc, how to make head turn ?

[UkuuXDMT322]

Hey, so i have been stuck quite a while now here.

Main problem is how do i turn mill head?

No way i have to change Z to sideways ?

And with multi axis "Rotary" is ment for turning stock, but thats not possible for me, since head can only move.

So with what tool can i make head turn , so it clears hole on right side of body.

When i changed Z direction, cnc went totally wrong direction.

Head can turn 90 degrees each way.

Thanks.

[engineguy]

@UkuuXDMT322 

Looking at your photo I think that your gantry moves away/towards you and is probably the Y axis, the Spindle moves Left/Right and is probably the X axis and the Head going Up/Down would be the Z axis.

Now, your Head will rotate around the Y axis so will likely be designated as the B axis so you won`t be able to use the full "Rotary" toolpath, you will need to set Angle Limits to suit the amount of degrees that your Head will move Left/Right from the Vertical position, for example Y -110 deg to Y+110 deg

You will need to have your Post Processor set to B Axis in the Y.

What Post Processor and CNC Control are you using, also can you upload your Fusion f3d file and a copy of the PP you are using so it can be checked for the Axis settings.

[UkuuXDMT322]

"Looking at your photo I think that your gantry moves away/towards you and is probably the Y axis, the Spindle moves Left/Right and is probably the X axis and the Head going Up/Down would be the Z axis."

Exactly.

"Now, your Head will rotate around the Y axis so will likely be designated as the B axis so you won`t be able to use the full "Rotary" toolpath, you will need to set Angle Limits to suit the amount of degrees that your Head will move Left/Right from the Vertical position, for example Y -110 deg to Y+110 deg.

You will need to have your Post Processor set to B Axis in the Y."

Well i changed rotation B axis onto Y axis and it made "simulation" better so that head now rotated like needed. With "Rotary" i run into problem, since tool is always facing towards centre of rotary, when i need to make holes on to side, its sideways.

Example :

"What Post Processor and CNC Control are you using, also can you upload your Fusion f3d file and a copy of the PP you are using so it can be checked for the Axis settings."

Well heres the story, since CNC machine we use, it seems to be quite "noname" probably was imported from china, and sold to us. Theres no name on machine. After some digging, im quite sure i found it:

https://youhaocnc.en.made-in-china.com/product/uwEacrgWsiYl/China-Youhao-4-Axis-CNC-Router-1325-2030... 

It uses LNC control system.

I called "dealer" and they said to use "HAAS" previous gen Post processing, so i have been trying to understand which one.

I got CNC "working"(edit:Moving) with 2 "HAAS" post processing, but i need to modify a bit code for it to work.

Our dealer site with the version we have:

https://www.deliverse.ee/delicnc-x700-4ex 

Ours table size is 2100x6000x350 if im not wrong, with 2 vacuums.

Edit: The drawings and manufactures i have made, are throwaways to learn how to make it move like i need. Tomorrow at work i will test it more.

Thank you.

[a.laasW8M6T]

you need to use tool orientation in the toolpath to select where you want your tool axis.

see screencast for an example

https://autode.sk/3QiFNm8 

[UkuuXDMT322]

Im using tool orientation, but with current setup and post proccesing, cnc couldnt read code, i had rotary axis set to B but on machine screen i saw A, so maybe thats the cause.

[a.laasW8M6T]

very likely if the post isn't configured correctly youre not going to get very far.

Can you upload the post processor you are using here?

and Confirm the rotary axis is The A axis and that it rotates around the Y axis.

Does the machine support TCP and/or Tilted work planes as this will influence the configuration too.

[engineguy · Accepted solution]

@UkuuXDMT322 

OK, changed to A axis around the Y axis 🙂 Image below of a simple test block that has a few different toolpaths just as an example, with a bit of luck this may be nearer for you 🙂 I have done a small Screencast of the Simulation and attached the Fusion f3d file and the Post Processor used for you to experiment with, have a look through the settings, may be of some help to you, would be better if you can upload the PP that you are using 🙂 🙂

Screencast link :- https://autode.sk/3eswbbl

[UkuuXDMT322]

Holy, you did so work to show me how its done 😁, i hope i wont own you anything 😊, but this really helped me, thank you so much, im gonna test it tomorrow and see what it does. About PP's im quite embarrased to show, because they are just stock files from fusion 360 library, Im quite sure "HAAS - Next Generation Control" and "HAAS (pre-NGC)" made CNC move, but only when i removed comments from code. But seriously your files and video help me learn alot. Will update tomorrow. Thank you.

[UkuuXDMT322]

Update: So i tried with engineguy's PP, it moves and it turned head 45 degrees, which is good. But cordinates and stock seem to be messed up. CNC thinks stock is 45 degrees or so, and X axis and Y axis go out of borders for CNC(so softlocks). I got the PP they use to cut in 2D but it works only with Aspire:

Spoiler

+ =======================================
+ ---
+ Version 1
+ Tony 10/08/2005 Written
+ Mark 03/06/2008 Added Arcs (no documentation).
+ Mark 09/02/2009 Added Toolchange
+ =======================================

POST_NAME = "LNC Arcs ATC(mm)(*.NCC)"

FILE_EXTENSION = "NCC"

UNITS = "MM"

+------------------------------------------------
+ Line terminating characters
+------------------------------------------------

LINE_ENDING = "[13][10]"

+------------------------------------------------
+ Block numbering
+------------------------------------------------

LINE_NUMBER_START = 10
LINE_NUMBER_INCREMENT = 5
LINE_NUMBER_MAXIMUM = 999999

+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]
VAR X_POSITION = [X|C|X|1.3]
VAR Y_POSITION = [Y|C|Y|1.3]
VAR Z_POSITION = [Z|C|Z|1.3]
VAR X_HOME_POSITION = [XH|A|X|1.3]
VAR Y_HOME_POSITION = [YH|A|Y|1.3]
VAR Z_HOME_POSITION = [ZH|A|Z|1.3]
VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.3]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.3]

+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"[N] G00 G21 G90 G54"
+ "([TOOLNAME])"
"[N] T[T] M6"
"[N] G00 [XH] [YH] [S] M03"
"[N] G43 H [T]"
"[N] [ZH]"

+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

+ "([TOOLNAME])"
"[N] T[T] M6"
"[N] G00 [XH] [YH] [S] M03"
"[N] G43 H[T]"
"[N] [ZH]"

+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin RAPID_MOVE

"[N] G00 [X] [Y] [Z]"

+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------

begin FIRST_FEED_MOVE

"[N] G01 [X] [Y] [Z] [F]"

+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------

begin FEED_MOVE

"[N] [X] [Y] [Z]"

+---------------------------------------------------
+ Commands output for the first clockwise arc move
+---------------------------------------------------

begin FIRST_CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for clockwise arc move
+---------------------------------------------------

begin CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J]"

+---------------------------------------------------
+ Commands output for the first counterclockwise arc move
+---------------------------------------------------

begin FIRST_CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for counterclockwise arc move
+---------------------------------------------------

begin CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J]"

+---------------------------------------------------
+ Commands output for a new segment - toolpath
+ with same toolnumber but maybe different feedrates
+---------------------------------------------------

begin NEW_SEGMENT

+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------

begin FOOTER

"[N] G00 G91 G28 [ZH]"
"[N] G49 G90"
"[N] G28 Y0"
"[N] M30"

[engineguy]

@UkuuXDMT322 

Going overtravel in X/Y will be down to your settings at the control, not a Fusion issue, whatever setup you use in Fusion you need the same at the CNC, without your Fusion file and how you have setup your WCS at the CNC not any way to diagnose so please, please upload a file that you want to run and it can be checked  🙂

The example file I uploaded should run OK but you must have the CNC setup correctly for this to happen, it should have moved to -90 deg and +90 deg with that program 🙂

[UkuuXDMT322]

I apologize, it was my bad, stock point was at wrong spot, the PP you supplied, it seems to be working, atleast was with swarf at 45 degrees, but with your manufactured detail, it gives error something with RIGTAP, no idea why.

So currently i have to try get right measurements for ISO 30 holder and right measurements for cutter, before trying with wood.

Im quite new to CNC so apologize for that🙂

[engineguy]

@UkuuXDMT322 

Ah, the Rigid Tapping error is my fault, should have thought that your CNC might not support that tapping, just use the "Supress" option to turn off the Tapping operations, or just delete them for now, you can experiment with Tapping later, the example file should then run without any errors 🙂

There is no real need to have the exact dimensions for a Holder, it is useful in the Simulation to check for Collisions but isn`t needed code wise, same goes for your Cutters, the important place for accuracy of the tools is at your CNC, if you want the exact same tooling dimensions in both your CNC and Fusion then measure your tools at the CNC first and then set your tools in Fusion to match, that way you will see a better representation in the Simulation 🙂

[UkuuXDMT322]

Thanks for info about holders, but how to i set lenght of tooltip to A axis? When i tried "Swaft", it rotates, but tool goes way too high. Seems that in simulation it rotates from top of tool, but A axis is way higher, how can i set that ?

[engineguy]

@UkuuXDMT322 

As I am not familiar with the tool and stock setup procedure for your CNC all I can do is show you a small example of two different Settings for your WCS, the main thing is that they must both be exactly the same in Fusion and your CNC.

In the attached example I have created two Setups in Fusion, one is set to the Bottom Center of the Stock and the second one is set to the Front Top Left as you would look at it, which is probably the easiest point on your Stock to "Touch Off" for your Part Zero and the top of the stock for your Tool Offsets.

If you run the Simulation you will see that the tool cuts exactly the same pass in both setups, which is correct.

However if you look at the generated code you will see that the X and Z values are different due to the different WCS selections.

So, if you set your WCS the same in both Fusion and your CNC then it should all work.

As I don`t have the Machine Extension I had to use a 2D Contour for the example, I left it at a single pass for clarity but in reality depending on material I would probably have used the "Roughing Passes" option, you can have a "play" with those settings if you are not already familiar with them 🙂

The first WCS image gives you the second image, the third WCS image gives you the fourth image, whichever point that you choose they must be set up exactly the same in both Fusion and the CNC 🙂

The example code is also below, note the difference in the X and Z values due to the different WCS selections.

%
O3032
(T1 D=10. CR=0. - FLAT END MILL)
N10 G00 G17 G21 G23 G40 G49 G80 G90 G94
N15 G28 G91 Z0 M19
N20 G28 G91 Z0
N25 G28 X0 Y0

(2D CONTOUR4)
N30 T1 M06
N35 G00 G90 S5000 M03
N40 G54
N45 G00 A-32.055
N50 M08
N55 G90 G00 X54.309 Y67.
N60 G43 Z64.916 H01
N65 G00 Z49.916
N70 G01 Z45.916 F333.
N75 Z18.218
N80 Y61. F1000.
N85 Y1.
N90 Y-5.
N95 G00 Z64.916

(2D CONTOUR4 2)
N100 G00 X48.208 Y67.
N105 Z-3.237
N110 Z-18.237
N115 G01 Z-22.237 F333.
N120 Z-49.935
N125 Y61. F1000.
N130 Y1.
N135 Y-5.
N140 G00 Z-3.237

N145 M09
N150 G28 G91 Z0
N155 G28 X0 Y0
N160 G49
N165 G00 A0.
N170 M30
%

Hope this helps 🙂

[UkuuXDMT322]

"As I am not familiar with the tool and stock setup procedure for your CNC all I can do is show you a small example of two different Settings for your WCS, the main thing is that they must both be exactly the same in Fusion and your CNC.

In the attached example I have created two Setups in Fusion, one is set to the Bottom Center of the Stock and the second one is set to the Front Top Left as you would look at it, which is probably the easiest point on your Stock to "Touch Off" for your Part Zero and the top of the stock for your Tool Offsets.

If you run the Simulation you will see that the tool cuts exactly the same pass in both setups, which is correct.

However if you look at the generated code you will see that the X and Z values are different due to the different WCS selections."

I Checked your examples, i guess easier for me is to Setup to bottom, then i can use already set G54, but i will keep your point on mind if i run into problems.

"So, if you set your WCS the same in both Fusion and your CNC then it should all work."

I guess you mean, lets say, in Fusion i put G54 and set up G54 on CNC so i can keep using that?

"As I don`t have the Machine Extension I had to use a 2D Contour for the example, I left it at a single pass for clarity but in reality depending on material I would probably have used the "Roughing Passes" option, you can have a "play" with those settings if you are not already familiar with them"

I really enjoyed to see, that different way to cut in a angle(no swarf). Didnt think about this way bymyself😁. + I looked how you put 2D Contour on, i was baffled, didnt understand how, so i went to Design and i saw you used something i didnt find anywhere and when i tried to edit that to see what is it, i was really lost. Maybe can you tell me what that is and how did you do that ? Thank you😊

I have to try playing with options at somepoint.

"The first WCS image gives you the second image, the third WCS image gives you the fourth image, whichever point that you choose they must be set up exactly the same in both Fusion and the CNC "

I guess with WCS i show CNC where Stock is from CNC Home point ? So which direction Stock is ?

Well im currently having problems with Z stays too high with Swarf when tool goes 45 degrees.

When A axis is 0 degrees and X axis moves, tool tip is at right depth(at table), when it does A axis turn (45 degrees), tool tip stays too high from table. Why is that ?

Well i tried to cut with 2D Contour also, but when i tried with CNC, it went out of CNC borders(softlock).

I inserted both version that i made, not exact but should be quite same as at my work, I didnt save file.

+ when i remade "Swaft" version and tried to Simulate, i spotted Z position to be really odd. Only happens on one side, but why ?

Thank you 😁

[engineguy]

@UkuuXDMT322 

I have modified your 2D Contour file, what I did was create  "Patchs" using the "Surfaces" strategy and just set them to 90 deg to the Model and used them for the Z axis Orientation, see History, quick and easy to do 🙂 File attached, image below.

I am not able to check your Swarf file as I do not have the Extension needed to Edit it, what I did see is the difference in Z height on the two ends, this is due to the different Angles used.

Your G54 must match in both Fusion and your CNC, unless you have a fixture that you place your Stock in so that the corner is in exactly the same position every time then you must re-set by probing/touching off the new stock for the G54 at the CNC every time for it to be machined in the correct position otherwise the Control doesn`t know exactly where the Stock is located, hope this helps 🙂

[ecastroCMJ5N]

As @a.laasW8M6T mentioned, most likely the problem lies on the configuration of the post. Since there is not a post available for your specific machine, you will have to do some edits to the "generic" posts provided in Fusion's post library. The recent post engine makes it actually very easy to create your own multi-axis post from the generic. Just take the time to read the relevant sections from the Autodesk CAM Post Processor Guide (Section 7). Some other useful sources for modifying the post to enable the 4th axis you can find here. Most likely your controller does not support TCP, so you will need to use the virtual tool-tip option on the post (which might be the culprit on why your Z axis seems off on your tests).