Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Fanuc lathe output tool call at each operation

10 REPLIES 10
SOLVED
Reply
Message 1 of 11
Metalyinsane
607 Views, 10 Replies

Fanuc lathe output tool call at each operation

Hello All,

 

I am not able to figure out how to modify attached Fanuc post to output tool call at each operation.

 

I have attached a debug file along with CPSv

 

(FACE2)
T#### (This should have a tool call in this position on every operation)
G40
G99
G97 S123 M3
G0 X515.922 Z10.
G50 S250
G96 S200 M3
G0 Z1.414
X511.921
G1 X512.75 F0.3
X509.921 Z0.
X358.4
X361.228 Z1.414
G0 X515.922
Z10.
G97 S123 M3
M9
G28 U0.
M0 (CHECK TOOL CHANGE)
M1

(PROFILE ROUGHING1 2)
N2 T0202
G54
G40
G99
G97 S179 M3
G0 X356. Z10.
G50 S250
G96 S200 M3
M8
G0 Z2.
X367.
G1 Z-46.8 F0.3
X360.
X358. Z-45.8
Labels (4)
10 REPLIES 10
Message 2 of 11
Anonymous
in reply to: Metalyinsane

I am not sure if this helps you but in my experience, if same tool is used in two or more consecutive operations, post only outputs tool call at the beginning of first operation.

Now, if I want to do 2 finish passes, stop after first one to check size and then run second pass, I have to input manual NC commands between the two operations using same tool.

First one is "stop", which outputs M0 and second one is "force tool change", which outputs tool call to second pass operation.

 

 

Message 3 of 11
Metalyinsane
in reply to: Anonymous

If the operator changes a wear offset and the tool is not called on repeat
of an operation the control doesn't adjust the offset or if the operator
goes back to old operation from another operation with a different tool the
tool is not called and the machine will crash.
Message 4 of 11
Anonymous
in reply to: Metalyinsane

Perhaps you missed my point, I was talking about scenario where same tool is used in 2 operations like 2 finish passes or rough and finish pass.

When posted Fusion outputs tool call at the top ONLY but both operations are one sequence with M1 at the end.

 

Now, if I want to stop between two operations and check size, adjust offset or scratch my back,...... next operation must have tool call as it is now separate sequence of program that runs independently of previous one.

 

In that case, I input manual NC between two operations and that results in tool being called in each one, I can manage that by manual NC withing Fusion or separate operations in NC editor after posting. and include tool call where needed.

Message 5 of 11
Anonymous
in reply to: Anonymous

Because there is a condition that determines whether or not tool is outputted on every consecutive operation using same tool, there is an option that you select to force tool change when and where desired,...... if so desired.

In attached file, post each setup and see the difference in output.

 

2020-12-08 19_48_37-Autodesk Fusion 360.png 

Message 6 of 11
bob.schultz
in reply to: Metalyinsane

@Anonymous's solution is the proper way to force a tool change on specific operations.  If you want to have a tool change on every operation the simplest method is for you to modify the post.  You can either force a tool change and the corresponding codes (G54, M08, etc.) on every operation by setting the variable insertToolCall to true at the top of onSection.

  var insertToolCall = forceToolAndRetract || isFirstSection() ||
    currentSection.getForceToolChange && currentSection.getForceToolChange() ||
    (tool.number != getPreviousSection().getTool().number) ||
    (tool.compensationOffset != getPreviousSection().getTool().compensationOffset) ||
    (tool.diameterOffset != getPreviousSection().getTool().diameterOffset) ||
    (tool.lengthOffset != getPreviousSection().getTool().lengthOffset);
  insertToolCall = true;  // <<< ADD THIS LINE

Or you can just output the Txxxx code on all operations without the other codes by modifying the following line where the Txxxx code is output in onSection.

  if (true /*insertToolCall*/) { // <<< MODIFY THIS LINE
    // onCommand(COMMAND_COOLANT_OFF);
  
    if (!isFirstSection() && properties.optionalStop) {
      onCommand(COMMAND_OPTIONAL_STOP);
    }

    if (tool.number > 99) {
      warning(localize("Tool number exceeds maximum value."));
    }

It is also easy enough to add a post property to control the output of the Txxxx codes if you do not want this behavior for every part.



Bob Schultz
Sr. Post Processor Developer

Message 7 of 11
Metalyinsane
in reply to: Anonymous

@Anonymous This is a great work around if people are not able to modify their post. Thanks for the input.

Message 8 of 11
Metalyinsane
in reply to: bob.schultz

@bob.schultz This is the solution I was after. Thank you for your advise. 

Message 9 of 11
Anonymous
in reply to: Metalyinsane

Manual NC is part of how Fusion works, not a workaround, what I do in many cases is using same tool to machine several features in a particular order. I want all of the operations to be posted using same tool and same offset, So if there are 5 operations in a row, all using same tool and offset but different depths of cut or feed rates, post outputs them as one sequence of program with assigned variables to each segment.

 

If I want to stop between any of the segments and clear chips or measure part, I insert "Stop" and "Force tool change" , that outputs M0 at the end of selected operation and new tool call at the beginning of the next operation using same tool and offset.

So my point is, tool call is managed for desired behavior depending on justification.

Manual NC allows me to manage that behavior rather than have redundancy and clutter all over NC program.



 

Message 10 of 11
Metalyinsane
in reply to: Anonymous

Yep, I agree with your method. But I have low information operators and
programmers and need to ensure simple solutions. Your method adds a margin
of human error which increases tooling cost and lowers throughput.
Message 11 of 11
Anonymous
in reply to: Metalyinsane


@Metalyinsane wrote:
Yep, I agree with your method. But I have low information operators and
programmers and need to ensure simple solutions. Your method adds a margin
of human error which increases tooling cost and lowers throughput.

Interesting analogy for flexibility that Fusion affords you for purpose of managing human error to your advantage.

Taking example of combining 5 operation that use same tool but different depth of cut or feed rate, you have a choice of posting it as one sequence of NC program or dividing it into 5 independent sequences, sending tool home between each one, subsequently increasing  demand on "low information operator".

 

Instead of operator staring at his phone while tool does the work, he has to observe all that stroking from home position to workpiece, if he needs to repeat any of the work, he has to be careful not to call wrong part of the program that can scrap part since there is nothing there to cut on repeat pass in specific area of the profile.

Machine uses excess lube oil, accelerates tear and wear, wastes time, annoys operator with needless stress which increases potential for error, … etc.😁

I am, however, in favor of pursuing personal freedoms of choice, just be aware of your choices and make the right choice when it matters.😎

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Technology Administrators


Autodesk Design & Make Report