Anilam generic post processor issues

[Anonymous]

Hello,

I have been having a hard time trying to get the generic Anilam post processor to work with my Anilam 1100m controller. Basically, I take the ".m" extension of the post and save it to a floppy disk so I can transfer it to the Anilam computer on my milling machine. From there, the machine will detect the disk and actually pull up the Anilam code in the editor and I can view it / edit it. But, when I try to do a run simulation or actually physically go for a cycle start, the machine will start to pull up "illegal" codes that is either a "$" or a funny looking "L" symbol stating that there are errors. From what I can gather, It must be a issue in the post processor script itself. But, I am not a programmer so I can only guess at what is going on here.

Anyway, until I get this problem solved, I have no use for Fusion 360 because my machine does not like the generic Anilam post processor. It seems that the post processor for Anilam may be about 90+ percent right, but its that small percentage that my machine does not like. My Anilam controller does not use spindle speed or a tool changer. It really only does the basic 3 axis milling work.

If anyone has any ideas for this kind of issue, I would be really thankful for the help. I can try my best to get whatever code or information that would be needed to help diagnose this problem. Until then, I have a 3100lb paperweight.

[HughesTooling]

Take a look at this post, I've attached a Anilam post there. You probably need to read the whole thread as well. There's an option in the post properties for the 1100m. Let me know if you have any problems.

Try the post attached to post #20

Mark

[Anonymous]

I was able to get my Anilam 1100m to respond favorably with the post #20 file you had mentioned. The only strange thing is that the Anilam control did not really appreciate the Mcodes. At line "8" it gave some spindle error that related to it being started at the improper time. Once I manually removed the Mcode from the conversational format, then the mill fired right up and ran its little face cycle without anymore trouble. Once the cycle was finished, the quill retracted to Z zero, tool zero and the spindle stopped on its own. I looked up the listing for Mcodes and it would appear that those codes are not absolutely nessesary for running basic 2.5D and 3D parts on a old Bridgeport mill. I guess the post processor gives the controller enough information to not require the Mcodes or something? My mill does not have a RPM encoder and my collant system is a hand operated ball valve.

Thank you very much for helping me with this problem I had! I have been scratching my head for several weeks trying to figure out what to do. I guess I will just have to manually edit the conversational code once it is in the controller. This is a lot better than where I was a hour ago.

[HughesTooling]

There are parameters to turn off the out put of RPM and coolant, try setting those to no and see if that helps. I have got an updated version, if I get some time I'll update the ones in that post.

Mark

[HughesTooling]

What M code number did you need to remove. Looking back I was asked to add the M3 for a 1100m control. If you need to get rid of the M3 try setting 1100m to no as well in the parameters on the post dialog.

Mark

[Anonymous]

I removed the M3 code. I believe it was on line 13 of my output conversational file. It seems that my Anilam control likes to have its tool detail manually inputed. So, when tool "1" is called out, then it just fires up the spindle according to the settings it reads on its tool page. If it has been running M codes, then it has never shown that to me in the program editor. The 1100M does have options in the tool page for coolant and rpm runctions, but my hardware does not take advantage of those extra features.

[HughesTooling]

When you post a file look through the parameters and set 1100m to no also RPM and coolant then you shouldn't get any m codes in the posted file. 

Mark

Edit thinking about it a bit more I seem to remember the 1100m could not handle modal arc movements, I'll try and add a setting to turn off the M3.

[Anonymous]

Yes, I just finished making the changes on the post processor screen and the M codes went away! Now I don't have to manually remove them once I upload the program to the control! This is great!

[kevin.brinklow]

Hi this maybe a long shot but do you still have a copy of the post processor file that

HughesTooling sent you 

it was the post processor for fusion 360 Anilam 1100m 

i looked at your post dated ‎12-10-2015 regarding the problem you had with error codes 

after you loaded a file from the floppy to the anilam controller

i am having the exact problem

did the post file that HughesTooling sent you work ok

have you still got it if so could you forward a copy to me 

best regards kev

[HughesTooling]

@kevin.brinklow Have read through this thread. The last post I attached in post#55 should work but read through the whole thread, it's quite a long time ago and can't really remember how it worked out for the 1100m control.

Mark

[kevin.brinklow]

Hi Mark thanks for the reply

i have had a read of the post & downloaded your latest post 

so i just down loaded the post into fusion 360 & posted my code to my floppy & loaded it onto the Anilam 1100m & hoped for the best 

selected the file from the list loaded the file pressed edit all good so far pressed the Draw option

then i am getting an ERROR Message when i try to draw the file

ERROR:  ILLegal  address 'A'

Draw canceled. 

any ideas 

 i must admit at this stage i am totaly lost when it comes editing post proccesor files so your help with this is very welcome  

Also i dont suppose you have a copy of the ofline software i could run on my PC  so i can try out my programs before i spend time loading them onto the machine

i have enclosed the (Contours file) that is giving me problems 

regards kev

[HughesTooling]

Do you know how to program the control manually? What I'd recommend is just program a simple rectangle using 2d profile and see if you can get it to work. If you can program the same rectangle manually you should be able to figure out what's different in the code Fusion's posting. I have a 3300m and not sure what differences there are between the 2 controls.

Also don't attach pictures, just paste them into the message or use the insert photo option. Can you edit you last message and embed the pictures to make it easier to read.

[kevin.brinklow]

 hi mark thanks for the update 

I will give your suggestion a go later today and let you know what the results are 

regards Kev

[kevin.brinklow]

Hi Mark 

i've got the anilam 1100m running with some basic code but i had to manualy edit out a couple of lines that were causing problems 

I have encloded the file for you to have a look at 

the lines that cause the 1100m to crash are

line   7    Mcode107

line 83   Offset Fixture# 0

can these be removed from the post proccessor  or will i have to manualy edit them out each time

the post proccesor that i am using is the Anilam conversationalModulV1.cps 

regards kev

[HughesTooling]

Does your control have fixture offsets? Not sure how to do safe tool changes if it doesn't.

I always use fixture offsets 1 to 9 and leave offset zero set to the machine home so I can recall offset 0 and go to Z zero for tool changes. I noticed in your code you have not set an offset in your setup, normally you'd want to set it to 1 or whatever offset you are using on the machine. Need to know if your control has offsets, might be the error is calling offset zero when that's to offset already active.

Ref M code 107. I use my machine for 2 axis work as well for drilling holes. M code 106 stops the control doing any Z moves similar to a dry run and 107 enables the Z moves. I just put the 107 at the start of programs to make sure Z moves are enabled so for you there's no problem removing that line.

Mark

[kevin.brinklow]

Hi mark
Thanks for the reply
I have looked through the user manual and have not found any information on fixture offsets
The machine has part offsets that you manually input before you run any code
I would normally put an extra line of code in the program when I want to do a manual tool change that takes the machine to X0. Y0. Z0 or to a safe area of the workpiece
The spindle automatically stops when a tool change is called so no worries there after the change has been made I just press the start button and the machine starts up and runs the code no problems
Also looking in the user manual I found some info in the appendix regarding Mcodes the anilam 1100 only supports
M3. M4. M5. M8. M9 very basic
So maybe that’s why it is showing up an error with the Mcode 107

Is it possible to delete the lines from the post proccesor that reference the fixture offset & also the line Mcode 107 so that the controller can’t see them
On a side note I had a play with my code & I found that If I delete the problem lines from the code on the edit screen the anilam runs ok all bar a couple of errors relating to radius size but the program completes

Best regards kev

[HughesTooling]

I haven't worked on this post for a long time but looking through it looks like line 315 needs commenting out to stop the M107, just put // at the start of the line.

Then at the bottom of the file comment out line 1108

Does going to Z0. retract the tool on your control? Do you have a powered quill or a powered table for the Z axis?

[kevin.brinklow]

Hi I will edit the post lines tonight as you have pointed out & see how that works
The quil is powered & has limit switches
Also the mill bed has limit switches on the X & Y
The Bridgeport was retrofitted by Anilam with the anilam 1100 controller back in 1997
Thanks again for the help I will get back to you with the update
Best regards Kev

[kevin.brinklow]

Hi Mark
i edited out the lines as highlighted that has done the trick
the only issue i am getting now is an error message that pops up when i run the program that message says

Circle Adjusted beyond Maximum Adjustment

the error does not stop the controller from running the program
is it possible to edit this out

regards kev

[HughesTooling]

---

@kevin.brinklow wrote:
Circle Adjusted beyond Maximum Adjustment

the error does not stop the controller from running the program
is it possible to edit this out

regards kev

---

No this can not  be fixed because the error is in the Anilam control! They are really not a good control and this error can and will scrap work like I mentioned in this post with an example backplot of the same code on an Anilam and Protrak control.

I really would not trust the control with anything much more complicated than a rectangle with rounded corners. Definity don't use it with a 3d contour toolpath if you've used smoothing. In the thread linked above I mention I added a setting to disable arcs and just output linear moves.

Mark