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)
4,051 Views
52 Replies
Replies (52)

daniel_lyall
Mentor
Mentor

You need to supply a lot more details a screenshot of the posted G code error or it, a file with this problem so on.


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

GeorgeRoberts
Autodesk
Autodesk

How are you setting the tool length like this? Are you setting the length with the head at 0, then rotating the head? 

 

The way you set this up will have an impact on how the post should output the code

 

-

George Roberts

Manufacturing Product manager
If you'd like to provide feedback and discuss how you would like things to be in the future, Email Me and we can arrange a virtual meeting!
0 Likes

engineguy
Mentor
Mentor
Accepted solution

@stanskimaciej 

 

Have you tried a simple 2D pocket and setting the PP as if it has 4th axis running in the "Y" ??

See image below and attached file, also G code that runs with no errors in Mach3 here, or try generating the code using your own PP :slightly_smiling_face:

Angled Slots.jpg

Angled slots pp.jpg

 

Might help point in the direction you want :slightly_smiling_face:

Stay Safe

Regards

Rob

0 Likes

stanskimaciej
Participant
Participant

This option Fourth axis mounted along Y is opening all options again, Thank you for that! I think i will take it from this point :face_with_tongue:

 

You totally get the idea what i want to do! 

 

Cheers !

0 Likes

mashcomDWK67
Contributor
Contributor

Hi @engineguy 

I have a similar problem. My spindle has been fixed to 90 degrees. In the NC file there is interpolation between the Y-axis and the Z-axis. The spindle, however, has been fixed to the Z-axis and the interpolation must be between Y and Z. I'm trying to repair the slot. I have attached a file of a door and a g-code.Inkedcnc router_LI11.jpg

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

Could do with some more information, never having used a CNC with that configuration I have to assume things :slightly_smiling_face:

 

1) When you switch over to your T2 spindle does your CNC control do a "swap axis" so that looking at your photo the Z axis now moves Left and Right instead of X and what was the Z axis with your T1 spindle becomes the X axis and the Y axis remains moving away from and towards you ???

 

If that is the case then we can possibly look at producing G code as if it is a 90 degree index move on a 4 axis setup.

Info please :slightly_smiling_face: :slightly_smiling_face:

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

Hi@engineguy 

The movement along the x and z axes is preserved at the two spindles T1 and T2. There is no swap axis option. The controller is Richauto A15.

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

So, you are saying that the whole head with both spindles bolted to it moves vertically and to be able to cut the slots in your door horizontally then to enter the material the it would be moving in the X direction and the cutting moves would be in the Y and Z directions ???

 

How are the two spindles started and stopped ? Do you have different M codes for each spindle ??

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

Hi @engineguy 

With T1 the first spindle is started, the second spindle is started with T2. The coordinate system of the first spindle is G54. The second spindle has two tools - left and right. The left one is operated with the coordinate system G55 and the right one with G56. The movements to the axes are always kept. It's a big problem because when working spindle T2, I have to change axis Z with axis X. Can that change be done in the postprocessors when starting T2? T1 and T2 are the tool numbers.

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

OK, so you need to have a T2 S**** command to start the T2 spindle instead of the usual M3 S**** command, that can be done I think, what Post Processor are you using and can you upload a copy of it with your next post ??

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

HI @engineguy 

This is how the first and second spindles start. I don't know how to choose the coordinate system in Fusion.Spindles.jpg

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

Right, it is the normal M3 S**** to start the spindle, the WCS setting G54/G55/G56 etc will I expect start the appropriate spindle so in the attached G code sample I have set it to G55 so the T2 spindle on the Left looking at your photo should start, see image below for where you set the G54/G55 etc, setting it to 1 is G54, 2 is G55, 3 is G56 and so on for as many as your control is enabled to handle.

Door 3 set WCS.jpg

Have a good look at the attached G code file, it moves in the Z axis down to level with your slot, and then moves along the Y and Z axis for direction of cut, it is a 2D Pocket and as the tool is only 12mm dia and the slots are 18mm and 16mm then the Machine Z axis will move up and down a small amount, the X axis is acting as a Z axis and moving deeper into the edge of the door which to me is all correct :slightly_smiling_face:

Hopefully this will get you closer !!

 

Anyway, see if your control will accept the code and gently try it out well above your machine bed :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

Usual caveat applies, use at your own risk :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

 

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

Hi,@engineguy 

 

How did you change the x-axis and z-axis values in the nc file?

0 Likes

mashcomDWK67
Contributor
Contributor

When I set different WS coordinate systems I get an error. I want the whole program to be in one file.WS problem.jpg

0 Likes

stanskimaciej
Participant
Participant

Hey sorry for late answer.  

 

I manage to make my machine working with 45 degrees tilted spindle. Main point was using other post processor. I try to attach my post to this post.... Its post processor made to work with 5 axis machine control by mach 3. But i remove tool offsets from turning axis so there is no compensation for distance from tip of the tool to rotating axis.

 

Usually when you turn your milling head tip of the tool is turning around your turning axis so post need to recalculate that. But in my case spindle is not rotating, its just attached on 45* angle. So i don't need compensation. 

 

Feel free to ask additional questions. Have a look on post. Try it if you are brave enough :face_with_tongue: 

 

If i would do project like you are doing i would for sure make one program for vertical spindle and separate for horizontal.  But of course if you are in production of many things you can connect them and use different WCS's.

 

 

0 Likes

engineguy
Mentor
Mentor

@mashcomDWK67 

 

The X and Z positioning are generated by the Post Processor that I used, which is the same one as @stanskimaciej  has attached to his reply, just download that one and copy and paste it into your Personal Post Library, see image.

Personal Post Library.jpg

Once you have that open scroll down to the "Open Folder", click on that and then paste the new PP into that folder, close that Posting area by clicking "Cancel", then re-open and you will be able to select that PP from the drop down list on the left where it is showing the PP I used, the 5AXISMAKER / 5axismaker - Copy4

 

I am puzzled, you said that you need a G55 to start your Left T2 spindle and a G56 to start your Right T2 spindle so you need to have multiple WCS for your control, the warning in your image is simply saying that you need to be using a PP that is enabled to handle multiple WCS :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

 

Hope you are nearer now :slightly_smiling_face:

Stay Safe

Regards

Rob

0 Likes

mashcomDWK67
Contributor
Contributor

Hi @stanskimaciej 

Thank you very much for the postprocessor. It seems it will work. Is it set anywhere in Fusion 360 that the X-axis and the Z-axis must be changed? I'll remove the offset of the tool as you mentioned.

 

Hi @engineguy 

Thank you very much. Why do I have to use G54, G55 and G56? What happened was that the controller does not support the offset of the tool but the X-axis has been displaced. I only set G55 0,0,0 and G56 0,-350,0 in the controller, so the vertices of both of the tools start milling from the original point. The situation is the same with the T1 spindle where there are different values for Y, X and Z. The controller supports 10 additional coordinate systems.

0 Likes

mashcomDWK67
Contributor
Contributor

Hi, @stanskimaciej 

 

The postprocessor of my CNC router works but when I change the spindles T1 and T2, T2 which has been set to 90 degrees touches the item. The CNC router  moves very slowly round the X-axis while the Z-axis moves fast, so that the tool touches the item. May I set the position to the Y-axis and the X-axis and then to set the position to the Z-axis to prevent the item from damaging?


(2D POCKET3)
M5
T2 M6
S15000 M4
G55
G90 G0 B-90. C-90.
G17
G0 X611. Y998.721  Z18.089
X601.
G94 G1 X597. F3203.
X584.7
X584.566 Y998.729 Z18.087
X584.433 Y998.751 Z18.084
X584.304 Y998.788 Z18.078
0 Likes

stanskimaciej
Participant
Participant

Can you send me access to your fusion 360 design? 

 

I dont understand entirerly what you mean by moving fast. Is it moving faster so its getting further then it should? Or its geting where it should by just too fast? Have any screencapture of some more info?

0 Likes