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

[lipscombrandy]

I can not open a cps file. is there anyway you can email me this is another format I can open? lipscombrandy@gmail.com 

[pdelioussine]

You should be able to open it with any text editor, as it is just an ASCII
text file.
For instance using notepad...

Open notepad
Go to File->Open
In the prompt change file type to " All files *.* "
Navigate to file location
Select post-processor you would like to edit
Just make sure to keep the .cps file extension when saving

With that said, you would be better off using something like Notepad++, as
it is far more feature rich when it comes to editing code.

[lipscombrandy]

Thanks. I’ve tried note and even photoshop but they won’t open. I use a Mac and not windows maybe that’s the problem. I’m super frustrated with the Anilam 3300m I’ve been at it for about 3 weeks and I can get the code into the system and even get it to run on the draw screen but when I try to run the part it’s all over the place. I can’t find anything that helps. Any help would be greatly appreciated 

[xr4x4ti]

Are there any updates on this post?  Is the generic Anilam post included in Fusion been updated to include the updates in this post?  

I am about to get an Anilam 3000M 3 axis mill and I am excited to try it out with Fushion 360.  

[lipscombrandy]

I had to use a totally different post processing cad program because fusion doesn’t post process the correct type of cad for Anilam 3300mk you’ll have to do so much work just to edit the code you may as well go back to the 80’s and write the whole program yourself. I’ve searched every post know to man and asked everywhere to get it to work. The easiest thing to do is just use a different program for the cam part and design your parts in fusion. 

[HughesTooling]

@lipscombrandy  Don't know what your problems are, I didn't reply before because you are using a mac and I couldn't help with that. The CPS files are just text and Notepad++ works great as an editor but it's not available for a mac.

The CPS files I attached to posts in this thread work fine for me but I've mostly used it for milling so not sure about the drill cycles. I never need to edit the code manually so not sure why you're having problems.

Mark

[lipscombrandy]

Thanks. I was able to open your file with note on my Mac but it’s so much work to edit the code to work with the older Anilam 3300mk that I just used a different cam/post process software and it worked perfect without any changes 

[HughesTooling]

I have a 3300mk that's about 20 years old and it works fine for me without any manual edits, what problems did you have?

Mark

[lipscombrandy]

It post processes a code that doesn’t look like anything that would work and it puts M’s in the code and the Anilam says code error and it doesn’t run correctly , it goes all off course when I run it and destroys parts

[lipscombrandy]

I generates a M in the code right after the speed and my Anilam reads that as a error. Ive tried to figure out how to get the post process to stop putting that M in there with no luck

[lipscombrandy]

Also when I remove the bad code and try to run the program it always goes to the machine home no matter what I choose for the work offset infusion. It’s pretty much just a mess. Are used a different post processing cam software and it generated code perfect the first time with no problems and ran all of my parts. I love fusion but their post processing for the Anilam 3300mk is horrible and I tried for a whole week to get it to run a part. 

[HughesTooling]

My machine doesn't have spindle speed control so I didn't notice that problem. From what I can see there should be a space after Mcode. So it should be Mcode 3, but I'm not sure you even need that. I set the direction in the tool table so just calling the tool starts the spindle. Is that the way you use the control? It's easy enough to mod the post either to output Mcode 3 or just remove completely. Same would go for the coolant code, should be Mcode 8, but 

I think part of the problem with the Anilam post from Autodesk is their software is quite new and the Anilam control is old, Anilam probably went out of business very early in the development of HSM and just didn't get much interest.

Mark

[lipscombrandy]

My machine doesn’t have spindle speed control either. I’ve checked in and checked every box in the post output to try to get it to stop posting the M code with no luck. Also even if I just manually erase it I can run the code but when I start the program in my machine instead of finding the home coordinates Of the part it always goes right back to the home coordinates of the machine no matter what and says soft limits reached

[HughesTooling]

Did you try the post I attached earlier in this thread? One thing I do that might be a bit different is call Offset 0 then go to Z0.0 for tool changes. I've used other CAM software that just goes to a fixed ABS position for tool changes but that's not good or very professional as you can run into the Z limit or have problems if tools have a big difference in length. Going to the machine limit will always give you the max clearance available.

I have found the problem with the MCode3 after a quick test. If you have the direction set in the tool table the spindle starts when the tool's called, then control then gives an error when the M3 is called because the spindle's already running. Most controls don't error if you have multiple M3s.

I'll upload another post in a while I've made a few more mods to. The way I work is I find the part zero, go to the offset page and zero XYZ for offset 1. In the setup in fusion I set it to use offset 1 as well, could use any other offsets of course just make sure they match. I leave offset 0 so Z0.0 is the machine limit, when the tool change is called the zero offset is called and Z goes to Z zero, after the tool change it called the current offset again and carries on.

When I start the machine I use the code below in the MDI to call up the offset I want and make it current so I don't adjust offset zero. Ignore line 5 that's commented out.

Mark

[HughesTooling]

Here's an updated post.

  
  outRPM: false,     // If true output RPM if false use machine tool table 
  SpindleMCodes: false, //Output M03 M04
  outCool: false,     // If true output Coolant on off if false use machine tool table 
  A1100: false,     // If true Anilam 1100 
  A3200: false,     // If true Anilam 3200 2 axis machine 
  AllowArcs: false, // If true output arcs
  quillDRO3300mk: false // Set true if machine is 3 axis and has a DRO on quill

A couple of changes from before. One SpindleMCodes, if true will output M3/4.

Second change is AllowArcs, for 3d work I'd set this to false. I've had several jobs scrapped because the Anilam control I have is crap! The problems usually happen if there are a lot of concentric circles like machining a hemisphere. 

Here's an example. As well as all the warnings you can see one circle way out of position.

And to prove it's the control here's the same OP posted to my prototrak without any errors!

Mark

Test the post carefully and I'd better add this 

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk.

Do not put custom posts in the generic posts folder. Use the personal folder, or another location. Or enable cloud posts and upload to the cloud assets posts folder.

Fusion 360 CAM Personal Posts Folder Locations

_______________________________________________________________________________

Microsoft Windows:
%appdata%\Autodesk\Fusion 360 CAM\Posts

Mac / Apple / OSX:
/Users/<user id>/Autodesk/Fusion 360 CAM/Posts

[lipscombrandy]

Awesome! Yea if you can post another file that I can try to run that would be great. I would really like to figure this out because I do love designing in fusion and I would love to do everything right off of their start to finish

[fireborn230]

Mark, you seem to be the leading authority on Anilam conversational posts.

I have a bed mill running a 3300m Anilam controller. I, like many of these other people, were very frustrated in trying to get code into my machine until I came across your post. So firstly, Thank you! My machine would not be running with code right now if not for you!

I have a few things that dont seem to be working in my post that maybe you can help with. The post does not seem to generate an M5 or "mcode5" before a tool change. I have to manually edit the code at the end of each tools code.(my tool changes are manual on this machine) I dont know my way around a post editor to save my life but I did find something that reads:

var mapCommand = {
COMMAND_SPINDLE_CLOCKWISE:3,
COMMAND_SPINDLE_COUNTERCLOCKWISE:4,
COMMAND_STOP_SPINDLE:5,     <----------------------This should be making the "mcode5" on tool change, no?
COMMAND_COOLANT_ON:8, // flood
COMMAND_COOLANT_OFF:9

Secondly, the real odd one is:  When I send out a program, it will run the program with no trouble but if I interrupt that program for any reason and want to restart that program, I get a Z limit on soft limit. If I remove the Z0 at the beginning of the program manually the program runs with no trouble.  Code as follows:

.5 CR=0 - ZMIN=-0.83 - FLAT END MILL

* TOOL 5  D=0.75 CR=0 - ZMIN=-0.83 - FLAT END MILL

* TOOL 6  D=0.201 CR=0 TAPER=118DEG - ZMIN=-0.3322 - DRILL

* TOOL 7  D=0.5 CR=0 TAPER=120DEG - ZMIN=-0.0991 - SPOT DRILL

Dim Abs

Plane XY

Unit Inch

Mcode9

Tool# 0

Rapid  Z0         <----------------This line seems to cause the issue, if removed it seems to solve the problem. Not                                                                   saying that's right.

* FACE1

Tool# 1

RPM 3000

Mcode3

Offset Fixture# 1

Mcode8

X3.8 Y-0.975 Z0.6

Z0.2

Line  Z0.17 Feed 48.

Plane XZ

Arc Ccw  X3.6 Z-0.03 XCenter3.6 ZCenter0.17

Line  X2.5

X-2.5

Plane XY

Arc Cw  X-2.5 Y0.031 XCenter-2.5 YCenter-0.472

Line  X2.5

Plane XZ

Arc Cw  X2.7 Z0.17 XCenter2.5 ZCenter0.17

Rapid  Z0.6

Plane XY

Mcode9

Tool# 0

Rapid  Z0

Currently running 7875_anilam conversationalModalV1 post downloaded from F-360 site.  your Please let me know your thoughts. Thank you!!

[Nicholasaltizer]

Im trying to utilize this post with rigid tapping on my Fryer MB10.  getting this error when attempting to post taping operations in fusion "Unsupported speed-feed synchronization" 

previous code looks something like this;

Tool# 3
MCode 6
Offset Fixture# 1
RPM 400
MCode 3
Rapid X0. Y0.
MCode 8Z0.1000
Tapping ZDepth -0.8375 StartHgt 0.1000 TPIorLead 20.0 SyncSpin Yes
X0. Y0.
DrillOff
Z1.0000