Need Post modification help

[M&GToolWorks]

I am trying to modify my Brother post to allow for in process broaching. I considered writing a macro to do this process, but with all the different variables for parts, I am not sure I could do it without spending a week on it. 

I am hoping to setup Fusion so that I can sketch out the coordinates I want to use relative to the part geometry. 

I started out with some reading and a couple posts here on the forum and found a link to this: https://chadkrause.com/blog/post/fusion-360-broaching

It is very helpful, except the code he shows does not match up with the code in my post. This is all done using the standard Brother post as I do not want to disturb my "tweaked" post. 

I have changed several aspects however get the following error: 

Error: Spindle speed out of range.
Error at line: 907
Error in operation: 'Drill2'
Failed while processing onSection() for record 347.

Line 902-907 read: 

if (!isProbeOperation() && (insertToolCall ||

        isFirstSection() ||

        (rpmFormat.areDifferent(spindleSpeed, getPreviousSection().getTool().spindleRPM)) ||

        (tool.clockwise != getPreviousSection().getTool().clockwise))) {

      if (spindleSpeed < 1) {

        error(localize("Spindle speed out of range."));

        return;

If I change those features (which doesn't seem like I would want to, as the probe should not be involved in this operation?) I get the following alarm: 

Error: The probe cycle 'probe' is machine specific and must always be handled in the post configuration.
Error in operation: 'Drill2'
Failed while processing onCycle() for record 363.

These are the only two sections that have "if (spindleSpeed < 1)" 

Any advise or input would be great. If someone has better guidelines for what to change to enable broaching, I am all eyes. 

Thanks

[Richard.stubley]

Hi @M&GToolWorks

What toolpath where you planning on using to mimic the broaching? 

Attaching the Fusion document too would be help in seeing how you are trying to do this.

[M&GToolWorks]

Currently I am using a drill cycle with rapid retract to make the bones of the program, then altering the program for my broaching.

Altering the code works, but I would much prefer to alter the post so that the code is usable. 

[Richard.stubley]

So if I've got this right you want to hijack one if the drilling cycles and use it as a drilling cycle?

Can you send over the code you want for broaching. I will try to put it in a drilling cycle.

[M&GToolWorks]

G54.1 P5

G100 G90 T01 X0.5321 Y0.0021 G43 Z0.6 H01 D01 

M08

G17

M19R45

G00 X0.5321 Y0.0021

G00 Z0.6

G00 Z0.2

G81 X0.5321 Y0.0021 Z-0.3392 R0.07 F155

X0.5328 Y0.0028

X0.5335 Y0.0035

X0.5342 Y0.0042

X0.5314 Y0.0014

X0.5307 Y0.0007

X0.53 Y0

G80

G00 Z0.6

This is currently how I have the code modified. I use the standard drilling cycle and modify it accordingly. 

The problem I am trying to fix is related to commanding a 0 rpm spindle speed. When a 0 rpm is specified it would be nice to have it output an M19 like in the example given in the blog referenced above. 

[boopathi.sivakumar]

@M&GToolWorks 

Hey already they have given way to modify the post. Did you tried that steps which is given in the blog?

if you didn't, try to modify the post as given in the blog

If you did try and getting some error kindly do attach the modified post so that we can take a look at it 

Also attach the model file as well so it will be helpful 

File>Export>.F3d
save the file and reattach the file to this thread.

[M&GToolWorks]

So I was able to work around the post and manually G code the section of code I needed. 

[banddspindles]

Where is this blog?

[banddspindles]

we broach everyday on our vmcs, draw a sketch with lines the length or step over i want per pass (60 passes at 0.003 per pass). So there will be like 60 small lines with .003 between lines(use pattern). I then select all lines in 2d contour and make sure the direction is correct (red arrow). This allows us to simulate it as well.

[M&GToolWorks]

Thanks for that, it is similar to what I wound up doing, except I sketched points and used a drill cycle. Will try it with the lines oriented in z with a 2d tool path. I didn't think to have them vertical. 

The blog is linked in my first post. 

[Richard.stubley]

Hi @M&GToolWorks

I've made a few mods and think I've got something that will work nicely.

So now you can specify a 0 spindle speed and it will work, I've added the property "allow 0 spindle speed"

Setting this to true will stop the error.

All you have to do now is place points at the positions you want to broach, create a drilling cycle and set the cycle type to custom. Set the speeds Plunge=broaching feed.

There is an additional property Broaching angle this lets you set the angle the spindle will be locked at. 

Yes the code is a bit lengthy as I've expanded the cycles but I fell its best to see whats going on.

 

Again please be careful and let me know how you get on.

[banddspindles]

The lines should not be vertical, they should be horizontal as in photo below. Also, be sure to get you correct m19 r value.  I use sub routines m98 to call my broaching operations and cancel with m99 to return to main program.