- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Rotary Plunges To Zero Position On Start
My Rotary is Axis A (4th Axis), I have my home position set to X0,Y0,Z0,A0.
Z0 is the middle of the stock on the Rotary, however I move the Z to Z40 for initial start position so its not burried in the material when moving to X0,Y0,A0 .. If that makes sense ..
The following code is generated by F360, using a Rotary Axis A (4th Axis).
However when I run the code, I believe at line 5 it plunges the spindle directly into the stock and tries to burry the cutter 20mm before any other actions.
1 (ANGEL - 42MM SQ - 1MM TAPERED - ROUGHING)
2 (T2 D=1. CR=1. TAPER=10DEG - TAPERED MILL)
3 G90 G94 G91.1 G40 G49 G17
4 G21
5 G28 G91 Z0.
6 G90
7 (FACE -135)
8 T2 M6
9 S10000 M3
10 G17 G90 G94
11 G54
12 G0 A135.
13 G0 X28.463 Y114.636
14 G43 Z32.757 H2
Fusion 360 lets me select Rotary when designing, which also sets the Zero points to the center of the stock.
Is this a programming error in F360, or is my machine somehow interpreting the code incorreclty ?
Is there a way in F360 to have the Zero Point set to the stock top, instead of the stock center ?
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
You don't say what post processor you're using. The line 5 G28 G91 Z0. is actually a move to the machine Z home position so if you've homed your machine it would go to the Z home.
If you're using the mach3 post there are options for safe retract if you don't home your machine.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hi, sorry, yes I am using Mach3 post processor.
I understand the G28 G91 Z0 is a move to home command ..
This tells the machine to go to Z0 1st, then proceed move to X0,Y0,A0 ..
I have found this code 8 times throughout the full program .. One for the beginning of each rotation movement ..
But why is it in the program, when the home position for my Rotary is 22mm below the surface of the material ?
How do I set a Z0 position to the top surface of the material, instead of the center of the rotational axis ?
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Edit.
@raptessmistfyre wrote:
Hi, sorry, yes I am using Mach3 post processor.
I understand the G28 G91 Z0 is a move to home command ..
This tells the machine to go to Z0 1st, then proceed move to X0,Y0,A0 ..
I don't think you do understand. The G28 is a move to the machine home (G53) not the part home (G54 or what ever offset you are calling).
@raptessmistfyre wrote:
But why is it in the program, when the home position for my Rotary is 22mm below the surface of the material ?
How do I set a Z0 position to the top surface of the material, instead of the center of the rotational axis ?
Does your machine have limit switches? You need to home your machine or set G53 X, Y and Z to a safe point, not sure how you do that manually, my machine has limit switches and the homing cycle sets the machine home (G53 is machine coordinates and G54 is the work coordinate system) automatically.
See this page for more info on G28.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
@raptessmistfyre wrote:
Hi, sorry, yes I am using Mach3 post processor.
But why is it in the program, when the home position for my Rotary is 22mm below the surface of the material ?
How do I set a Z0 position to the top surface of the material, instead of the center of the rotational axis ?
IF you have no limit switches and no machine home position set there is an option on the post dialog shown in my first reply to use the clearance height. I would still recommend setting a home position though and use G28 as that is the safest option.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
My machine does not have limit switches.
I understand the 'Home' position for the machine is where I move the spindle to and set it to X0Y0Z0A0.
This is how I have been doing it for 3 years or so now, and its been working just fine with Vcare & Aspire using wrapping technique.
In Aspire, I unwrap the mesh into a 2.5D model. Set the 'Home' point to the surface of the material. Wrap the X axis to the A axis. Presto, it mills ... With 'ok' details, but misses anything that is slightly off the vertical line, that you can only get with multi axis milling.
As for Fusion 360 and currenet issue, I tried setting it to 'Clearance' mode in the post processing, but this just returned errors. I did get it to work with a single surface process, however if I added the 45 degree rotation for the 2nd surface, the errors returned saying the retract will not clear the material (or somthing like that).
This also does not let me set the Z0 to the surface of the material.
I know I'm new to F360 .. But at this rate, I'm going to be bald in a few weeks .. lol
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Ok, further testing done .. Still no solution ![]()
When using the 'Clearing' mode on Post Processing, it gives an error for any machining that is done at any angle other than Zero .. So this method is not an option for rotary toolpath ..
Error: Safe retract option 'Clearance Height' is only supported when all operations are along the setup Z-axis.
Error at line: 1139
Error in operation: 'Face 90'
I have attached the actual file I am trying to process, If you (or anyone) is willing to take a look at it and see if I have done something wrong, or if you can tell me how to change the Z0 from Rotary Center, to Stock Top, or anything else that may help in resolving this problem ..
The extra strange thing about all this, is that I have already used a previous version of this task and it worked just fine. Although I had a different (wrong) tool selected for it and since I changed the tool to the correct one and then regenerated the code, it hasn't worked for me since ![]()
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
You haven't told us what type of machine you're using, You should have some type of machine origin (Home) to relate to.
Please read what, and follow the link that, @HughesTooling posted.
There are hundreds of posts in this forum that relate to your problem, it's not a Fusion related problem or a bug.
/David
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Easiest thing to do is Re-connect the machine with Z at its highest point. On my GRBL controller, it sets this as machine 0 if there are no switches.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
I have a CNCest machine, bought on eBay many years ago. It runs a Mach3 controller of Chinese origin, I have upgraded the drivers to digital ones .. Other than that, I can tell you no more details.
It does not have limit switches, Never have I needed to set a Machine Home position, I've always just moved the spindle to the starting point of material surface, zeroed all the axis and pressed start ..
It's always worked in the past this way and it's only been since I started using F360 that I am now having an issue ..
I do understand it's not F360 that is the problem.
I don't understand how to get around or work with the G28 command ..
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Ok, so correct me if I am wrong (again) ..
Machine Home is set when I power the CNC on, to the current XYZA positions ? ..
This is seperate from where I set the XYZA Zero position when setting up for a job.
G28 command, refered to Machine Home and Not the Zero I set ..
G28 will move to Machine Home, then proceed to the starting position set in the milling code ..
So as long as my Machine Home is set away/above the stock, it will not cause crashes into the material when G28 is called ?
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
G28 command, refered to Machine Home and Not the Zero I set ..
G28 will move to Machine Home, then proceed to the starting position set in the milling code ..
So as long as my Machine Home is set away/above the stock, it will not cause crashes into the material when G28 is called ?
Correct.
Found a video for you:
https://www.youtube.com/watch?v=zFk_U3yqrks
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
@raptessmistfyre wrote:
Ok, so correct me if I am wrong (again) ..
Machine Home is set when I power the CNC on, to the current XYZA positions ? ..
This is seperate from where I set the XYZA Zero position when setting up for a job.
G28 command, refered to Machine Home and Not the Zero I set ..
G28 will move to Machine Home, then proceed to the starting position set in the milling code ..
So as long as my Machine Home is set away/above the stock, it will not cause crashes into the material when G28 is called ?
This is correct and a lot safer than using a relative offset above the stock. If you have tool changes (change from a short tool to long) you can make sure the longest tool clears using G28 where you could have problems using part offsets.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
@raptessmistfyre wrote:
I have a CNCest machine, bought on eBay many years ago. It runs a Mach3 controller of Chinese origin, I have upgraded the drivers to digital ones .. Other than that, I can tell you no more details.
It does not have limit switches, Never have I needed to set a Machine Home position, I've always just moved the spindle to the starting point of material surface, zeroed all the axis and pressed start ..
It's always worked in the past this way and it's only been since I started using F360 that I am now having an issue ..
I do understand it's not F360 that is the problem.
I don't understand how to get around or work with the G28 command ..
You really should look at fitting limit switches so you can home the machine. If you have a fixed home you can re-reference the machine if it loses position plus you can recall offsets (G54, 55 etc.) and leave jigs\fixtures set up. The switches are in series so you only need 3 switches and a bit of wire, hopefully your controller has connections for the limit switches.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Fusion