Fusion
Community
I set the post up so Tool# 0 is maximum retract to the Z limit switch and set all offsets from there. One way you could work around would be to have a holder as tool zero touch the job and zero, move up to a safe point that clears your longest tool and zero again then set your offsets from there. Working from the limit switch or safe point is a lot easier and safer than hard coding a Z height because of the problems you can have with tools with very different lengths.
Matk
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.
I set the post up so Tool# 0 is maximum retract to the Z limit switch and set all offsets from there. One way you could work around would be to have a holder as tool zero touch the job and zero, move up to a safe point that clears your longest tool and zero again then set your offsets from there. Working from the limit switch or safe point is a lot easier and safer than hard coding a Z height because of the problems you can have with tools with very different lengths.
Matk
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.
I'm pretty sure moves are modal even between programs, so if the last move in a program is a Rapid it not canceled. Can be dangerous if you stop a program half way through.
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.
I'm pretty sure moves are modal even between programs, so if the last move in a program is a Rapid it not canceled. Can be dangerous if you stop a program half way through.
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.
That code is pretty common for lots of controls, but all Anilam users are taught to use that format. I assume you're not using tool length offsets, but instead setting zero at the top of the part. Most people set zero at the fully retracted position and then offset the tool down to the part. So canceling the Tool Offset (Tool 0) and then moving to Z0, will move the quill to a safe zone, above the part.
This is the same way I program my Anilam control (Anilam 1100, which is the same format as the 3000 series control).
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
That code is pretty common for lots of controls, but all Anilam users are taught to use that format. I assume you're not using tool length offsets, but instead setting zero at the top of the part. Most people set zero at the fully retracted position and then offset the tool down to the part. So canceling the Tool Offset (Tool 0) and then moving to Z0, will move the quill to a safe zone, above the part.
This is the same way I program my Anilam control (Anilam 1100, which is the same format as the 3000 series control).
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
I found the Anilam gave even more trouble using R, did you just change the option in user parameters to yes.
In the Anilam control there's an option for a tolerance for arc errors, there are 2 options, move centres or move endpoints. Anilam's advice is to set it to move endpoints which is terrible advice, if you move the endpoint you will not reach the programed position.
Here's an example of move endpoints ending up 0.05mm out of position, X should be -15.00.
The problem using R is the arc tolerance allowance in the control has no effect. I don't know why Anilam had so much trouble getting arcs working, they tried to tell me the problem was the CAM's not accurate enough. When I told them it ran on my Eztrak, Heidenhain and Charmilles wire eroder they stopped wanting to talk to me. One final note on the tolerance setting, it doesn't change to match the units the control is running in, I think it's set to 0.005", if your control is set to mm it stays set to 0.005mm not 0.012.
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.
I found the Anilam gave even more trouble using R, did you just change the option in user parameters to yes.
In the Anilam control there's an option for a tolerance for arc errors, there are 2 options, move centres or move endpoints. Anilam's advice is to set it to move endpoints which is terrible advice, if you move the endpoint you will not reach the programed position.
Here's an example of move endpoints ending up 0.05mm out of position, X should be -15.00.
The problem using R is the arc tolerance allowance in the control has no effect. I don't know why Anilam had so much trouble getting arcs working, they tried to tell me the problem was the CAM's not accurate enough. When I told them it ran on my Eztrak, Heidenhain and Charmilles wire eroder they stopped wanting to talk to me. One final note on the tolerance setting, it doesn't change to match the units the control is running in, I think it's set to 0.005", if your control is set to mm it stays set to 0.005mm not 0.012.
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.
@szkiXHQG3 wrote:
Thank you That has solved most of the processor problems I have been having.
Have you ever had the mill have a command to move x y and z and it have an error of radius not found it is only the first modal move line I can put (rapid) in front works every time I can put (line) in front works. Another thing I commonly do is just erase the z value since the line after it has a z value. The funny thing is sometimes it will work fine for a few runs of the program then it will find it as an error. In my above example it is this.....
Tool# 1
X-3.5015 Y0.9278 Z0.6
Z0.16
Line Z-0.009 Feed 15.
@szkiXHQG3 What post gave this code and can you share a Fusion design that gives this error. Export the design and save as an f3d. I've never seen that happen, the only thing I can think of is the control is still set to an arc move, is this the modified post?
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.
@szkiXHQG3 wrote:
Thank you That has solved most of the processor problems I have been having.
Have you ever had the mill have a command to move x y and z and it have an error of radius not found it is only the first modal move line I can put (rapid) in front works every time I can put (line) in front works. Another thing I commonly do is just erase the z value since the line after it has a z value. The funny thing is sometimes it will work fine for a few runs of the program then it will find it as an error. In my above example it is this.....
Tool# 1
X-3.5015 Y0.9278 Z0.6
Z0.16
Line Z-0.009 Feed 15.
@szkiXHQG3 What post gave this code and can you share a Fusion design that gives this error. Export the design and save as an f3d. I've never seen that happen, the only thing I can think of is the control is still set to an arc move, is this the modified post?
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.
Accepted solution
@szkiXHQG3 Give the attached post a try. I've added a parameter to the post, ZHome. Warning test carefuly and be careful because the CAM will not know where you've positioned the Z.
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.
@szkiXHQG3 Give the attached post a try. I've added a parameter to the post, ZHome. Warning test carefuly and be careful because the CAM will not know where you've positioned the Z.
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.
"Warning test carefully and be careful because the CAM will not know where you've positioned the Z."
I understand that you might be using just 1 tool. So it seems easier to just touch off of the top of the part and set zero. But you should consider just putting in a 1" Tool Length Offset and touch off of a 1" block. In the long run it is safer ans still allows for a TLO adjustment at the machine. Just my .02¢ From a guy who used to work for Anilam teaching their programming classes.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
"Warning test carefully and be careful because the CAM will not know where you've positioned the Z."
I understand that you might be using just 1 tool. So it seems easier to just touch off of the top of the part and set zero. But you should consider just putting in a 1" Tool Length Offset and touch off of a 1" block. In the long run it is safer ans still allows for a TLO adjustment at the machine. Just my .02¢ From a guy who used to work for Anilam teaching their programming classes.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
However I do plan on downloading the post to see what you did and how you did it. Thanks for your efforts to make these changes. I hope it will be a learning experience for me.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
However I do plan on downloading the post to see what you did and how you did it. Thanks for your efforts to make these changes. I hope it will be a learning experience for me.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
@mike.mattera wrote:
"Warning test carefully and be careful because the CAM will not know where you've positioned the Z."
I understand that you might be using just 1 tool. So it seems easier to just touch off of the top of the part and set zero. But you should consider just putting in a 1" Tool Length Offset and touch off of a 1" block. In the long run it is safer ans still allows for a TLO adjustment at the machine. Just my .02¢ From a guy who used to work for Anilam teaching their programming classes.
Yes Mike, I wouldn't use a post like this. I work off the machine Z home like you described, I suggested the same. But it seems @szkiXHQG3 is pretty determined to stick with the way he's been working and just removing the first Z move from the post is even more dangerous!
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.
@mike.mattera wrote:
"Warning test carefully and be careful because the CAM will not know where you've positioned the Z."
I understand that you might be using just 1 tool. So it seems easier to just touch off of the top of the part and set zero. But you should consider just putting in a 1" Tool Length Offset and touch off of a 1" block. In the long run it is safer ans still allows for a TLO adjustment at the machine. Just my .02¢ From a guy who used to work for Anilam teaching their programming classes.
Yes Mike, I wouldn't use a post like this. I work off the machine Z home like you described, I suggested the same. But it seems @szkiXHQG3 is pretty determined to stick with the way he's been working and just removing the first Z move from the post is even more dangerous!
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.
@HughesTooling Mark, do you have an Anilam control too?
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
@HughesTooling Mark, do you have an Anilam control too?
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
@mike.mattera You might want to read through this post, I made some pretty big changes from the generic post. Support told me conversational posts couldn't have modal moves, I like a challenge and they were wrong.
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.
@mike.mattera You might want to read through this post, I made some pretty big changes from the generic post. Support told me conversational posts couldn't have modal moves, I like a challenge and they were wrong.
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.
@mike.mattera wrote:
@HughesTooling Mark, do you have an Anilam control too?
Yes but the experience has not been good. I guess the control programmers were as good as Fanuc and Heidenhain but too many people between the users and the programmers. The UK managing director didn't want to listen to the problems I had and the salesman just stared at his feet looking rather embarrassed. Sorry for the rant!
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.
@mike.mattera wrote:
@HughesTooling Mark, do you have an Anilam control too?
Yes but the experience has not been good. I guess the control programmers were as good as Fanuc and Heidenhain but too many people between the users and the programmers. The UK managing director didn't want to listen to the problems I had and the salesman just stared at his feet looking rather embarrassed. Sorry for the rant!
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.
Sounds like you're a fan of the Heidenhain control also. IMHO one of the most sophisticated controls on the market. Powerful macro language. I used to teach Heidenhain programming when I worked for Hermle Machine.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
Sounds like you're a fan of the Heidenhain control also. IMHO one of the most sophisticated controls on the market. Powerful macro language. I used to teach Heidenhain programming when I worked for Hermle Machine.
Mike Mattera
Fusion Content Experience Designer - CAM
Getting Started In Fusion CAM | Introduction To 2D Machining | Interface Fundamentals | Keyboard Shortcuts
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
