Looking For Siemens Acramatic 2100 Post Processor For Fusion 360

Hello All!
I am looking for a Siemens Acrmatic 2100 post processor for Fusion 360. The generic A2100 post processor requires too many edits to make it of much use. I have an old post processor from another CAM software that works fairly well, however it does not work with F360. I was hoping someone had an A2100 post processor they use that they would be willing to share? Or maybe looking for someone who knows how to make/edit post processors? I have all the programming books, some good programs I currently use, and edited A2100 post processor I found online(for F360, but just isnt correct, but works better then the generic). This control is quite complex from the Meldas M3, Fanuc 6, and Haas controls I use in my shop. But this A2100 control is actually quite nice to work with once I figured it out. Thank you in advance.

Can you place the edited post and some good code in a Zip file and upload it here so someone can have a look at it for you.

So I am going to attach a few different files here. All of these posts are machining the same part. A 5"x7"x2" with 3 1" holes in it. I mill the outside with a 1/2" Mill. I helix the center hole with a 1/2" mill. I plunge center of hole, and mill contour of center hole with 1/2" mill. I spot drill all 3 holes. And I peck drill through all 3 holes.



The First file +MPA2100E is a post processor from my old Cam software that I am most happy with of the processors I have dealt with.



The second is 1250C MC9. This is the post generated from using the above mentioned processor.



The third is 1250C MC9 Edit. This is the same above post with the edits that I do to make it run smoothly. I need to change the beginning order of each program a bit. I also need to change the ending and start of each operation. I need to add an H# and Z# in my starting position line with spindle start. The H# is the work offset, similar to G54, G55, this uses H1, and H2 and so forth. I also need a Z dimension in this line. It can be any dimension, but it needs to have a Z position. It could be the initial Clearance height. The drilling cycle has minor changes to it. R# can be zero as the control adds .1" as default to the retract height. R is actually hole surface positions. W# is the jump height between positions. If it is set to non existent or .1", it will be the same as that is dimension from zero plane, and as it already has a default R of .1", it will jump .1" between parts. The K value is the peck depth. Z is the depth to drill hole from ther R positions. So if you have a part that is 2" thick. And a pocket 1" deep with a hole in that pocket that goes through part. You would need an R-1., with a Z-1. to drill to the bottom of 2". Then you use a W1.1" to have the tool jump to 1.1" above the R value, so would then be .1" above the top of the part. At the very end of program I have added an H2 position, that is just a position I use to bring the table to front center of door. If I am running 4 vices(which I do run quite frequently), I will set the H5 value to my load postion. This line is NOT needed, but is kinda nice.



The fourth file is 1250C F360 No R Arcs. This is posted with the default Acramatic 2100 processor in F360. The box is not checked to use R Arcs. As you can see it uses I's, J's, and K's. That isnt the biggest issue. The main issue is just the overall formatting of the post. I need to have (MSG, xxx) in order to have messages. Pretty much everything about the formatting isnt quite right in comparison to my previous posts.



The 5th file is 1250C F360 R Arcs. Same as post above, but with the use R arcs box checked. As you can see it sill does not use R arcs. Still using I's, J's and K's. Also, this machine can use P arcs, but I notice every post I have ever used in this control has been with P's instead of I,J,K. Looking in the manual. IJK is for contouring, while P(R) is used to put a Radius on the corner of a part, or C is used for a chamfer on a part. I guess technicall you can switch IJK for P without issue.



The 6th file is Acramatic-CZ. This is an edited processor I found online.



The 7th file is posting above F360 program through the Acramatic-CZ processor, 1250C F360 Edited.

There is a way to make the helix program shorter, and that is to just remove all of the middle. The helix does not need to be broken into quadrants. If you have the K(z dimension per revolution) and the Z(final depth of helix), it will helix at that angle all the way till it hits the final Z depth. That would shorten it a lot.

All the F360 posts are just off. The drilling adds an R.1, then also adds a .1" to the Z dimension to make up foe the raise in the R value. However I see that as a band aide and would rather have it be R0. and Z-2. Running production that extra .1" of drilling can add up. especially when you are only drilling a 1/4" part, your adding nearly 50% drill depth. I also mentioned in my initial post that Fusion would not post a helix for this machine. However when I made this test piece to make sample posts, it seems to have decided to work. Not sure why it wouldn't work before. I am also going to add a few pages from my Acramatic programming manual for reference. I hope this all makes sense? If theres any questions, feel free to ask. Thank you in advanced.

hi, this would be best to do one step at a time, for fusion 360... no use posting other stuff... so what is the first step you would like done the most... keep it simple.. this is confusing as it is ... was this posted in the fusion forum..?

Its hard where to start lol I guess maybe can we start with the Start of the program? Start at the top and Ill work my way down. Ill work with the default Fusion 360 processor as everyone can get theyres hands on it. I have posted this to the F360 forum for post processors. I hope this is what you mean by keeping it simple?

Currently the Fusion 360 Processor posts this as the start(adding tool and machine write)
: (PGM, NAME="1250C F360 R Arcs")
; T1 D=0.5 CR=0 - ZMIN=-2 - FLAT END MILL
; T2 D=0.3937 CR=0 TAPER=118DEG - ZMIN=-0.1 - CENTER DRILL
; T3 D=0.5 CR=0 TAPER=118DEG - ZMIN=-2 - DRILL
: G90 G40 G94
G17
G70
M26
; CONTOUR

Im hoping to change the header to this
(PGM, NAME="1250C F360 R Arcs")
(MSG, T1 D=0.5 CR=0 - ZMIN=-2 - FLAT END MILL)
(MSG, T2 D=0.3937 CR=0 TAPER=118DEG - ZMIN=-0.1 - CENTER DRILL)
(MSG, T3 D=0.5 CR=0 TAPER=118DEG - ZMIN=-2 - DRILL)
(MSG, CONTOUR)

Once I work past this step, I will move onto operation headers which is where (MSG, CONTOUR) will start.

edited line 116 and 137...check it out, If I am correct, the Arrow 750 I have runs good on that acramatic-CZ.cps, it needs the " ; " for comments... file 2 is the one ...attached..

That change did work great! And it changed every comment through the program and not just the start. So a few steps further. When I first received this machine 5 years ago, I remember there being A LOT of small issues I have had with the programs and how they were written, so i have found a way to post them and not have issues. Maybe you are right in the I dont need (MSG, xxxx) in order to run the program. But back when I was first learnig this machine I have stuck with it. Maybe thats all I tried. Maybe I tried your way and it didnt work. I honestly dont remember lol But the Programming manual says to use (MSG, xxx), so now I use it that way haha Onto a few more changes if possible if you dont mind?

Two are a setting in F360. When I use the CZ or CZ2 post, F360 does not allow me to use letters in the Program name/number. If I use the default Acramatic post in F360, it does allow me to use letters. Not sure if thats a simple change in the post or not? Also, another setting that may be easily changed, to un check the box that defaults to preloading tools. This machine does not preload tools. These 2 things are small issue that I can easily work around.

Onto actual changes to how it posts. Maybe I can get the start of a milling operation changed? Here is how the CZ2 posts.

(PGM, NAME="00001")
(MSG,T1 D=0.5 CR=0 - ZMIN=-2 - FLAT END MILL)
(MSG,T2 D=0.3937 CR=0 TAPER=118DEG - ZMIN=-0.1 - CENTER DRILL)
(MSG,T3 D=0.5 CR=0 TAPER=118DEG - ZMIN=-2 - DRILL)
: G90 G40 G94
G17
G70
(MSG,CONTOUR)
M9
:T1 M6
S1400 M3
M8
G0 X0.25 Y-5.75
Z0.4
Z0.1
G1 Z0.05 F50
Z-2
Y-5.5 F10

This is how I would like it to look. I changed the beginning of these a bit, this way allows me to start the program at any operation and it will read all settings it needs. Currently if I start at "(MSG, CONTOUR)", the machine would alarm out as it hasnt read ":G17 G40 G70 G80 G90 G94". So if my contour operation is in the middle of my program, it ould not run if I searched for the contour operation. The M8 is moved up as it takes a few seconds for coolant to actually start flooding the tool, and the machine is faster then the coolant, so i need to give coolant that extra head start. I need to have an "H#" added in the X#Y# line, this is used instead of G54.
(PGM, NAME="00001")
(MSG,T1 D=0.5 CR=0 - ZMIN=-2 - FLAT END MILL)
(MSG,T2 D=0.3937 CR=0 TAPER=118DEG - ZMIN=-0.1 - CENTER DRILL)
(MSG,T3 D=0.5 CR=0 TAPER=118DEG - ZMIN=-2 - DRILL)
(MSG,CONTOUR)
:G17 G40 G70 G80 G90 G94
:T1 M6
M8
G0 G90 H1 X0.25 Y-5.75 Z.4 S1400 M3
Z0.1
G1 Z0.05 F50.
Z-2.
Y-5.5 F10.

I cant thank you enough. Even for the changes you already made withe the (MSG, xxx) lines. Having to change every one of those lines adds up. I wish I knew code. When I look at these post processors in word, I just see a jumbled mess of characters. I give you a lot of credit to be able to understand this. And I do see the changes you made too. I looked at both files. I try to learn things when I can. If someone makes a change to something, I try to see what they changed and understand it. Thank you again.

preload tools is line 40, change the true or false...use visual studios editor for editing...

Thank you. I am in the process of getting Visual Quick Code Set up and also gonna read through the F360 Post Processor manual. I did find the pre-load tools line. I also found program name as integer, which will allow me to use letters as well. I found these by using Microsoft Word lol I will have Visual Quick COde set up today or tomorrow.

Okay. So I have been working with VSC to try and understand what is going on inside the post processor. I am starting to understand it. However I am still having trouble how to execute what I want. Here for example. I have a line that is currently posted one way. And I would like to make it posted a slightly different way.

Here is the before Processor

// absolute coordinates and feed per min
writeBlock(":",gPlaneModal.format(17), gFormat.format(40), gCycleModal.format(80), gAbsIncModal.format(90), gFeedModeModal.format(94));

switch (unit) {
case IN:
writeBlock(gUnitModal.format(70));
break;
case MM:
writeBlock(gUnitModal.format(71));
break;
}
}

Here is the posted line from the above processor
: G17 G40 G80 G90 G94
G70

What I am looking to do is to add my G70 into the line above it. However, being that the G70 is a switched code, I cant find a way to add the G70 and leave it switchable to the line above. I highly doubt I will ever use G71 as I run everything in IN, but, I have OCD and like to keep options open if possible lol I just like to have the 1 line that has all the code I need. It makes the program cleaner and shorter. One thing that sucks about the A2100 control is I can only see like 8 lines at a time while machine is running. 2 of which are previously read lines, 1 is the line currently being run, then the following lines are lines coming up to be read. Like I said though, its not very many, so if I can remove wasted line and combine as much as I can it will make running a program and reading program while running easier so you know what to expect during set up.
: G17 G40 G70 G80 G90 G94

I apologize for bumping old threads but I'm trying to spread some knowledge that is hopefully helpful to anyone searching for a fusion 360 acramatic post processor.

I have a working post-processor that I'm adding probing & 4th axis functionality to. I'm using it on a sabre 1000 but I suspect it'll be closer than most of the vickers posts that are floating around for any of the acramatic controlled units.

I'm happy to take any and all feedback or changes - https://github.com/JeremiahChurch/acramatic_2100_fusion_360_post