Anilam conversational post FIX

[HughesTooling]

Edit 03/03/2015 updated attachment see latest post for changes.

I've fixed a lot of errors in the Anilam post.
List of changes.
IJK needed to be output as XCenter, YCenter and ZCenter.
Added helical moves all planes.
Added spiral work around to reduce code size.

Work offset 0 recalls the machine home, change so only 1 to 9 are output. If 0 offset is used in the setup in HSM no offset is output so whatever offset the machine is set to wiil be used.

No modal output for planes or moves. Added 2 new functions "writePlaneBlock()" & "writeMoveBlock()" to replace G-code with the correct Anilam words.

Fixed drill cycles. XY coordinate are not on the same line as cycle set up, moved to next line. No dwell in drill cycles changed to use boring cycle. Fixed chip breaking and deep drilling to correct format.
Set start and return to same height and ZDepth to cycle.bottom

Added quillDRO to properties if you have 3 axis and a coupled DRO on quill set to true and program will pause so you can retract quill before move to Z home.

Changed M code output so it outputs "Mcode"

Commented out RPM output as it's set in the tool table on the machine. When I have time I'll put a setting in properties to make easier changes.

Changes in post are commented with "HT" and date.

I've tested what I can, if you spot any problems let me know.

Mark

[HughesTooling]

Ok had to sort this out so here's a new post. If you set useRadius to yes the post will linearize spirales. From my tests on a 3d pocket this increased code size from 580 lines to 930 line so if you can I'd set useRadius to No.


Mark.

Edit also added Helical moves when useRadius = Yes.

[fishtruk]

Hi Mark,

Here's a link to the drawing in Fusion 360.

https://myhub.autodesk360.com/ue29ff914/shares/public/SHabee1QT1a327cf2b7a8625619612db9018

Nelson

[HughesTooling]

Hi Nelson

Did you try the post uploaded on May 22, it seemed to work for my control. Also have you tried using circle centres instead of radius.

Mark.

[fishtruk]

Hey MARK,

With Radius set to No it works fine.  Do you have any idea why it was erroring out?  It always happened in a lead-out from the cut - but when I crunched the numbers they were all good...

I think F-360 should hire you.

Now I have to look for a generic G-code post with no frills for my Camsoft driven machine. I don't think I saw one in F-360's small number of posts.. I'm surprised they had an Anilam post there...

Thanks Again,
Nelson

[fishtruk]

Hey,

It seems the Fanuc Generic does the trick. I assume anything Fanuc is liable to be the most generic but I don't want t make an "ass" out of "u" and "me"...

[HughesTooling]

fishtruk wrote:
Hey MARK, With Radius set to No it works fine.  Do you have any idea why it was erroring out?  It always happened in a lead-out from the cut - but when I crunched the numbers they were all good...

The lead-outs are spiral moves if you post a small file using the dump post you will see these moves have a start radius and an end radius. I've modified the post so that if the start\end radius are within a tolerance an arc is used. It looks like the Anilam control has tolerance settings for acrs using circle centre but it's not working for Radius. The file I tested had a spiral with a start radius of 0.7mm and an end radius of 0.70024 the control didn't complain using circle centers but stopped when using R!

Mark.

[fishtruk]

The file I tested had a spiral with a start radius of 0.7mm and an end radius of 0.70024

Mark,

Where did you get the .70024?

When I said I crunched the numbers, I got the start point from the code, drew that point in Cad, then drew an arc to the next XY based on the "bad" line of code. It all seemed to work out. Am I missing something?

I don't understand the path between a drawing and the G-code. The posts I've seen just address the syntax of the cutting machine. I don't know the steps CAM does before the post rules are applied. I assume it makes a point to point file based on the machining strategy then sends it thru the post "filter"

My brain hurts.
Nelson

[Anonymous]

A small note for anyone having issues with arcs doing weird things on the machine:
Be sure that in the Control Software Setup (on the controller), "Circle Adjustments" is set to End-Point and "Circle Centers" is set to Modal.
I spent some hours trying to figure out why the post wasn't working. Fortunately Jerry at Heidenhain knew about this issue. Any chance this could be added as a comment in the postprocessor?

EDIT: This was on an Anilam 1100 controller, not a 3000 series. I wonder if this has something to do with it?

[HughesTooling]

Where would you want it. Do you want it as a comment at the start of the posted file or just a note in the postprocessor.

Mark.

[HughesTooling]

Just a note on setting the "Circle Adjustments" to endpoint. To me that seems a bad idea as you will lose accuracy, imagine you are machining a square 100mm square with rounded corners and for some reason the control can't make the arc fit so it moves the end point there's a chance you won't get a 100mm square. Moving the center of the is not as important, the arc might be out a small amount but all the endpoints will be correct so the square will have parallel side and be dead square.

On my control I have adjustments set to Centre and a tolerance of 0.03mm, I get some warning errors but none that stop the machine.

Mark.

[HughesTooling]

I just run a test on the difference between moving the centre point and endpoint, and moving the endpoint is not a good idea.

Here's an example where I changed the circle centre form X-10 Y-10 to X-9.95 Y-10 just to force an error.
As you can see with adjust end point instead of reaching X-15 Y-15 you only reach X-14.95


Here's what you get with move circle centre. The arc might be out a bit but at least the path passes through X-15 Y-15


I've attached the file, if you simulate with single step you will see the error continues around the profile and would probably scrap your job.

Mark.

[Anonymous]

I'm going to do some additional troubleshooting. The issue we were experiencing was that the arc toolpaths would make large circles, often exceeding the X/Y axis travel of the machine. It's possible this is only due to one of those settings, but we will need to troubleshoot.

I should add, this was on an 1100 controller, not a 3000 series, so the software may be slightly different.

[HughesTooling]

I just had a problem with some arcs in the YZ plane not working so I had a look through the manual and found all the default setting seem to assume you are working in inches. Max arc correction is 0.005" when you change the default units it doesn't change so I changed it to .012mm and changed the internal accuracy to 0.00001 and external to 0.001 and the program runs without error.

I've run a few tests just to check the accuracy and it seems ok, so if you're running in millimeters this might be the problem.


Mark

[zomie1]

Howdy There,

I actually registered just to say thank you for posting this post processor!   It has saved my bacon.   I have noticed a few items.

When I try to do drilling it doesn't do chains.  It only does the first hole.   Also sometimes it seems to skip the first hole.  Any ideas on that?

Great work again!   I just got a bedmill that uses a 3300m and I was worried after running the generic post processor I was either going to have to write my own, modify the existing or just get mad and convert the machine to mach 3 🙂

All the best,

[deruiterwill]

Has anyone managed to get this working with a 3000m. Tried various thinks posted in the thread with out luck.

[pdelioussine]

Attached is a post processor I have been using on a Anilam 3000M bed mill, based on the work of HughesTooling.

Some of the changes include: Modal Fixutures, Tooling changes, Coolant. Additionally the output file is formatted in a way that is easy to read in a text editor.

Important notes:

The modal fixtures still need some work, they do not always restart the spindle.

I have not had too much time with this specific post, so just to be safe I suggest skimming through the output code.

More updates coming soon...

Best,
Peter

[Anonymous]

Mark, 

I am using an anilam 1100m and found this post processor extremely helpful.  

The entire thread helped me get up and running.  

Peck drilling is also not working for me but its on my list of things to do.  

I made a change to remove the moves to Z0 at the beginning and end of the cycle if anyone else needs this version just PM me. 

@Anonymous   Your post helped me end a day of banging my head on the wall.  I didn't mess with the adjustments but found the setting for circle centers was set to incremental instead of modal.....  What a difference that one setting can make  🙂

If I can get a version with a working peck drill cycle maybe I will post it.

[alistairjcook]

Good morning, I have an Anilam 3000m controller and trying to run a program that I have generated using fusion. I have designed the part and inserted the correct tool paths etc, used the 300m post processor file that is mentioned about however, when I go to load the program on to the controller via floppy disk it comes up with page error in the top left hand corner and crashes the controller? Any thoughts?

Cheers
Alistair

[HughesTooling]

@alistairjcook Did you find a fix for your problem, lost track of this thread so didn't see your question. Are you seeing the problem with all files even something simple. Page error sounds like a memory problem so a small file might load.

Mark

[Anonymous]

Hello Mark,

I've been following the thread on Anilam conversational posts over the last year, and I'm very grateful that you shared your work through this forum.  I bought a milling machine with Anilam 1100 software, but have resolved not had time to sort out using the cnc mode until now.  As it works well in DRO mode, I've made do with that.

I have tried creating a CAM output files for the mill, but I seemed to have particular issues loading lines for curves Arc Cw etc.., it just missed them completely.

So I had a closer look last night, I had been using the Generic Anilam Conversational post  version 41369, but I found the translation at  var xOutput = createVariable({prefix:"X "}, xyzFormat);   was putting a space betwen the axis and value, and that's what the 1100 software didn't like.  Removing the space has resolved that issue; quite a relief.
 
A fairly recent enquiry from fishtruk about a post for his Anilam 1100 had a reply that suggested going to the Post Library.  In the official area for Anilam, the current post is Anilam ISO, a Generic milling post for Anilam ISO (revision 42145).  The extension on this is 'nc', rather than 'm', and to my eyes the sample code shown doesn't look very conversational.  It also misses the options to turn off RPM and coolant commands, which my machine does not support.

So I'm thinking I would be better using your suggested post modification - I think 9106 was your most recent offering, which seems to include the options pertinent to the needs of the 1100; does that make sense, or should I be using something else ?

Thanks,

Rob