Anilam Post Processor Problems, Chevalier 1418 vmc-40

[greggor.mcgrath]

Hello everyone,

I was hoping someone may be able to shed some light on how I can resolve the error I am getting which I have provided below. I recently picked up a Chevalier 1418 vmc-40 an older model but in great condition and runs on an Anilam 6000M controller. The error is referring to my last operation on the part which is tapping. I have tried multiple tapping choices within the "cycle type" within fusion to no avail. 

Thank you!

Error: Unsupported speed-feed synchronization activation command.
Error in operation: 'Drill6'
Failed while processing onCycle() for record 6308.

[boopathi.sivakumar · Accepted solution]

@greggor.mcgrath 

I think you are using tapping with chip breaking i hope,

Anilam post processor is not configured with tapping with chip breaking cycle,

if you want to use then have to modify the post,

If you have any sample code for how you want, you can post the codes it here  i will take a look at it.

[greggor.mcgrath]

@boopathi.sivakumar 

Hello and thank you for your reply. I'm actually using "Right tapping" in the cycle type and have also tried "tapping", and tapping with chip breaking and still get the same error. Unfortunately fusion will not post any of the code for me to look at because of these errors. I have 9 total operations and they all work without error with exception of the tap operation.

[boopathi.sivakumar · Accepted solution]

@greggor.mcgrath 

What is the post processor you are using is it Anilam ISO or something else.

Can you check this post whether you are getting the output Post Library Analim

because the generic is already configured with tapping cycle.

If you are using some customized post then attach to this thread,make sure .zip the file before attaching

[greggor.mcgrath]

@boopathi.sivakumar 

Thank you so much! I installed the post you sent me and now I am not getting any error and it completed giving me the G-code. Originally I was using the Anilam Conversational within the Fusion 360 Post Processes section.

I really can't thank you enough for your help and very appreciative for such a quick solution. Because I have an older machine I thought I may not be able to resolve this very quickly.

Thank you again 🙂

[greggor.mcgrath]

@boopathi.sivakumar 

Hello once again. I just wanted to update you and let you know how the post worked. First off thank you once again, I was successful in running the program however I did have to make a few changes to the program blocks. When calling for a tool for instance block N15 T1 M6  calling for my face mill, the very next block would call for N16 T2 putting T1 away and grabbing T2 so I immediately stopped the program . I noticed at each tool change I would receive a call out for for the correct tool followed by the next tool in line putting the correct tool away and using the wrong tool for the operation. So what I did was remove the uncalled for tool change in each tool change section of the program and this corrected the issue. I also received an error of "invalid address D" this is what the block N3169 format was for the error. "N3169 G41 X4.204 Y-1.8602 D2 F25" I removed the D2 along with the Tool change issues and boom, everything worked perfectly. 

I just wanted to share these errors with you in case it may be useful in the future.

[boopathi.sivakumar]

@greggor.mcgrath 

You have the control to not post the next tool by disable the preload tool to false in the post properties

this will allow you to not post the next tool and

to disable D from posting you needs some post editing open the .cps file search for this portion

case RADIUS_COMPENSATION_LEFT:
        dOutput.reset();
        writeBlock(gMotionModal.format(1), gFormat.format(41), x, y, z, dOutput.format(d), f);
        break;
      case RADIUS_COMPENSATION_RIGHT:
        dOutput.reset();
        writeBlock(gMotionModal.format(1), gFormat.format(42), x, y, z, dOutput.format(d), f);

remove the dOutput.format(d), from both the lines it will allow you to not post the D in the program.

You need not delete every time in the NC.

[greggor.mcgrath]

@boopathi.sivakumar Hello again, I was hoping you may be able to assist me once again. Since I have talked with you last everything with the post has been working well however with one exception. After the end of a program the spindle does not shut down. The X Y Z return home however the spindle has to manually be shut down. I have done some research on how to edit the post however I'm a bit afraid to try it as I am unsure just exactly where to add the M5 G-code. I would also also like to spindle to orient its self "M19" after it shuts down. I have tried making edits to the code after its posted, then save to my chip followed by installing it to the machine however the machine does not recognize the change.  Thank you for any help you may be able to provide.

[etorres289KT]

how can i change the feedrate output, ej; 500rpm and 20 ipt this is equal to 25.0 g84x0.y0.x-.5r.200f25.0

. but my controler does not like that,

i checked their tapping sample and it shows g84 x0. y0.z-.5 R.200f20 s500 so feedrate is actually TPI