Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Milling pockets on 45* angled with mill head on 45* angle.

stanskimaciej
Participant

Milling pockets on 45* angled with mill head on 45* angle.

stanskimaciej
Participant
Participant

Recently i have ordered additional accessory for my CNC. Its Adapter plate to install spindle on 45*angle. 

 

stanskimaciej_0-1602061018156.png

And now i have to mill cabinet doors with vent slots on 45* angle. 

stanskimaciej_1-1602061092124.png

I Have good results with programming Swarf strategy, its look almost like it. But i cant get g-code out of fusion. It spits out some bits with failed notification. Machine is running on mach3.

stanskimaciej_2-1602061218484.png

I was trying as well 3d pocket with tool orientation but first of all i think is not what i should by using. Because Its changing WCS. Movement (Z) up and down in slot should be interpolated movement of Z and X axis when tool is at angle, if i get it right.  And this 3d pocket i cant get generated post processor as well

 

I kind of spend some hours on that problem and at the moment i have no more ideas. Need to go back to productive work for a while, I will get back to it in few h. If someone have some ideas would be great.  

0 Likes
Reply
Accepted solutions (1)
4,036 Views
52 Replies
Replies (52)

mashcomDWK67
Contributor
Contributor

Hi @stanskimaciej 

 

Please look at the attachment, the T1 spindle drills the two holes, then it changes the spindles T1 and T2. At this time T2 is above the door. T2 must go to the initial position. G0 X705. Y919.209 Z17 makes the spindles move on the three axes. Before the X-axis reaches the position X705 the Z -axis reaches position Z17. This leads to milling of the door.

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

This closer to what you need?

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

Forgot image :slightly_smiling_face:Door D v3.jpg

0 Likes

mashcomDWK67
Contributor
Contributor

How can I change the postprocessor so that it moves along the x-axis and the y-axis first. After reaching the position on the x-axis and on the y-axis, the spindle should be lowered on the z-axis.

That's right now

(2D POCKET2)
M5
T2
S8085 M4
G54
G0 B-90. C-90.
G17
G0 X705. Y919.209 Z17.
G94 G1 X607.5 F3203.
X602.5

 

Can the code be changed to:

2D POCKET2)
M5
T2
S8085 M4
G54
G0 B-90. C-90.
G17
G0 X705. Y919.209   I want it to reach the x-axis and y-axis points first

G0 Z17.
G94 G1 X607.5 F3203.
X602.5

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

Try attached PP

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

@engineguy 

Thank you very much, I will try it. I saw that in the manufacturer's postprocessor for the three axes use the command G43. Do you think it is good to use this command to ensure the retract height of the tool.

 

Retract.jpg

(2D POCKET2)
M5
T2
S8085 M4
G54
G0 B90. C90.
G17

G0 X705. Y919.209
G43 Z55. H1- Tool Length Compensation

Z17.
G1 X607.5 F3203.


0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

For me personally I always use the G43 command, if the Tool Library in the CNC Control has been correctly set with all the tool offset lengths then it is a much safer way to work IMHO :slightly_smiling_face: :slightly_smiling_face:

 

I also like to have the G28/G53  commands in operation, means more machine movement but again much safer :slightly_smiling_face: :slightly_smiling_face:

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

I personally tried with the G28 command activated and there was no change in operation, the machine did not observe a safe height of movement. I see a parameter in your postprocessor "safe retract distance", but I don't see

how it affects the g-code?

Safe.jpg

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

That is a distance that is used when a part is rotating in a Multi Axis machine, it is added to the Tool Length Offset to make sure the tool retracts far enough to be clear of the part when the part rotates.

 

Doesn`t apply to your machine as there are no rotational moves, don`t bother with ti :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

@engineguy 

Now when I look at your post processor, some of the loops actually use retract height. Only when the spindle is rotated is this information lost.

 

(2D CONTOUR3)
M5
T1 M6
S15000 M3
G54
G0 B0. C0.
G0 X-3.8 Y-1.6
Z55. retract height
Z45.
G1 Z36. F75000.

 

(BORE1)
G0 X535.5 Y1051.6
Z55. retract height
Z14.
G1 Z13.6 F2397.
G18 G3 X533.9 Z12. R1.6

(2D POCKET2)
M5
T2 M6
S8085 M4
G54
G0 B90. C90.
G17   Missing Z55
G0 X705. Y919.209
Z17.
G94 G1 X607.5 F3203.
X602.5

0 Likes

stanskimaciej
Participant
Participant

I think this problem is more then i can solve but i try to follow you guys. 

 

I have some additional question to make situation for me clear. Do you actually try this setup and program already? Is it milling everything correct but just when its swap from T1 to T2 its jogging to start position thru part and destroy it? but then carry on in correct order and do exactly what it should by doing?

0 Likes

mashcomDWK67
Contributor
Contributor

Yes, after moving the shingles T2 to the milling position, there is no problem. When the cycle ends, the spindle is shifted to the set offset T2. If spindle T2 is positioned above the door and I start the program, spindle T2 touches the door. My CNC router has a problem moving to the starting milling position, it moves the spindle on all axes. The side channel for the door lock is 1/2 of the thickness of the door. In my opinion, it must first reach the position along x and y and then position it along the axis z.

 

 

CNC router12.jpg

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

Thought we had fixed the start moves to be

X705. Y919.209

Z17

as you asked for ?? Does it not work ??

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

No, no change again rests on the detail. Is it possible to introduce a safe distance of 160 mm in the post processor, whenever the spindle is tilted at an angle?

For example:

(2D POCKET2)
M5
T2 M6
S8085 M4
G54
B90. C90.
G0 X615. Y922.709 Z160.  The distance should be fixed 160 mm
Z17.
X605.
G1 X603.699 F3203.
G2 X602.5 Y923.867 R1.2
G1 X596.524 Y1095.

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

You must have you Machine Z0 setting wrong, in the generated code there is no Z axis movement until it gets to the Z17.

There is an X and Y value one one line and the machine will execute that line first so it should be at the

X705 Y919.029

then goes to

Z17

Can`t be wrong, simple commands !!

 

There is a G54 in the code before those lines, do you have any values set for that in your machine.

 

Where do you set your machine Z0, not the Part Z0 but the Machine Z0, if you have Limit Switches that you machine homes to that is where your machine should be before it starts to run any G code so if it is up at the top of the Z axis travel then it should execute the X705 Y 919.029 line of code at machine Rapid speed before it does any Z axis moves.

 

If do not have any Limit Switches you should jog the machine to a safe position in all axis, set that position as your Machine Home in all axis and the code above should work correctly.

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

When I combine, the operation of the two spindles in one program becomes the problem. I always have to move the spindle outside the door. There must be some distance added in this case 150-160 mm when moving the spindle T2. At the first spindle T1 if I remove Z55. retract height, also the tool rests on the door.

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

If you machine accepts either a G28 or a G53 command then that can be used to move the Z axis up to a safe area, is this the case ??

0 Likes

mashcomDWK67
Contributor
Contributor

For some reason, the controller does not work with the machine coordinate system G53, accepts positions only relative to G54, I tried G55 and G56 if you remember I wrote, but it turned out that the controller works only in the one I chose when running the program. This controller despaired me despite the fact that the manufacturer claims that it supports G28, G53, G54 .... G59

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

OK, if it won`t play nice and the manufacturer isn`t being very helpful then we can try inserting the Z160 height instead if the G28 so try this PP and leave it to the default of no G28 at point of posting, it is outputting a Z160 at the points where there would have been a G28, so now the machine when Homed either automatically or manually when the code starts to run the machine should go straight to Z160 (Can make it 200 if needed, depends on how much Z travel you have) before it goes anywhere else, then at the end of every operation it should move to Z160 before moving to the next operation as normal, if it is the same tool it will just use the Height setting for the Retract as always.

 

Hope this is getting nearer, you must be getting really frustrated :disappointed_face: :(:(

Doing it as quick as I can, not best at modifying PPs :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

Hi @engineguy 

Thank you very much now the tool does not touch the door. I think you can increase the distance on the g28 to 200mm, for greater security, but it still works for now.

0 Likes