Felder Multiaxis Operations Post Processor

[josefloresb]

Hello,

I'm having some issues when I'm trying to do a multiaxis program for our Felder Profit H350 machine.
I modeled a very simple object to do a test:
Model

I want to do a swarf on that chamfer:

Everything seems fine when I do the simulation in Fusion 360, but when I post process the program I only get this code:

TPA\ALBATROS\EDICAD\01.00:74:r0w0
$=1001
::SIDE=0;
::UNm DL=121 DH=121 DS=20
VAR{
}VAR
OPTI{
}OPTI
SIDE#0{
W#1110{ ::WT2 WF=1 WS=1 #8098=..\custom\mcr\iso.tmcr #8500=0 #8501=0.iso #8502=0 #8504=0 #8505=1 #8520=1 #8522=1005 #8551=1 }W
}SIDE
SIDE#1 {
$=F #1
}SIDE
SIDE#3 {
$=F #3
}SIDE
SIDE#4 {
$=F #4
}SIDE
SIDE#5 {
$=F #5
}SIDE
SIDE#6 {
$=F #6
}SIDE

I'm not sure if something is missing in the post processor or if I'm missing something.
I'm using the Felder Post Processor found here: https://cam.autodesk.com/hsmposts?p=felder_profit

Thanks in advance!

[boopathi.sivakumar · Accepted solution]

@josefloresb 

All the 5 axis moves will be posted out as a sub program and it will be in the same location of the main program you choosen with the name of 0.iso , 1.iso etc.., based on the number of operations you are posting

[josefloresb]

Hi @boopathi.sivakumar 

Thank you for your response. I hadn't noticed the iso files. 
However I just did a test and the CNC moves the head to the entry position and then it does nothing. What I mean is that it rotates the head while aproaching the piece and once it gets there, it gets stuck, it doesn't move and it doesn't end the program.

I attached a video with the issue.

Thank you!

[josefloresb]

I just did another test, I manually changed the feed in the ISO files to F8000 and it is working great now.

Even though I have it configured in Fusion 360 to 8000 mm/min the output in the ISO file is between F3.81 and F10.
The head appeared to be stuck because it was moving really really slow.
How can I change the post so it outputs the ISO files at the correct speed so I don't have to change it manually?

Thanks @boopathi.sivakumar 

[josefloresb · Accepted solution]

I figured it out.
I changed the lines 218 and 220 of the PP from:

// calculate output feed rate in Meters per Minute
function getFeed(feed) {
  if (unit == IN) {
    return (feed * 25.4) / 1000;
  } else {
    return feed / 1000;
  }
}

to:

// calculate output feed rate in Milimeters per Minute
function getFeed(feed) {
  if (unit == IN) {
    return (feed * 25.4);
  } else {
    return feed;
  }
}

Thanks again

[Anonymous]

Hi there, 

I have been trying to figure out this post-processing with Felder post processor as well and it's a nightmare to be honest. Is there any way that the Multi-axis toolpath could be made to output into a .tcn file just the same as other?

The current way it means having to copy the ISO file to the sub folder on the CNC, which is a separate folder where the CNC board looks for the sub programme. The issue is that you cannot open in in TPA cad to edit if you have issue with anything. Also having two separate files for toolpath output makes it quite time consuming and more or less unworkable in the long run. You cannot change the file name unless editing the tcn file generated in notepad. All this seems rather counterproductive and makes generating 5 axis toolpaths so tricky 😞

But most importantly having the same issue as previous comments with the feed. The tool goes into position and then does not move. If it was output into tcn file you could then load it in the machines CAD and check it. 

Would you guys be able to look into making this post processor work for Felder CNC's please?  I was super excited to try to use Fusion 360 for true 5 axis work and at the moment it seems like mission impossible :(( Thanks a lot for your efforts. Otherwise enjoying designing with this software and would love to use it fully for machining. Hope you can help. Thanks a million. Pavel 

[Anonymous]

Hi there, posted a comment below. Would you guys be able to look into this for us? 5 axis work isn't working at the moment. Thanks a lot 😉

[alexeletel]

Hello,

I have a Felder H350 as well and I am having the same problem when using 5-axis tool paths. Any luck figuring out anything new in the past couple of months? How were you able to load the sub program onto the CNC because my sub program saves as a disc image file and the file name is 0. I do not have much experience editing post files but I would like to get this working.

Also, I noticed that the drilling toolpath does not save the tool number after posting so I have to manually enter the tool number for each hole in the machines CAD. Which is time consuming and counterproductive for what we are doing.

Any help would be very much appreciated. Thanks 

[Anonymous]

Hi I have a Felder H500 and have only just found out that Fusion has the post processor. I ve never done any machining through fusion as I have always used Alphacam Ultimate. I would be really interested if any of you guys out there have used or still use alphacam but are now using fusion instead and is it any better.

I want be able to set up machine styles for machining doors etc. can it be done in fusion and will it update if you alter sizes etc. 

Just a little side note on the 5 axis stuff. I believe the way the post works it has to post out separate .iso file and this has to be placed in the product folder which is in users/format4. The .TCN will be read directly from TPA cad onto the machine board when you load the program but if the .ISO is not in product folder it will not find it and the program will not work.

Sorry if you already knew this just thought it might help if not.

thanks 

Paul

[Anonymous]

Hello mate,

I'm having an awful time with this ... any chance you could screenshot the post process window to show the .iso file the way it should be written?

I'm attaching the simple file I'm trying to run bellow

[alexeletel]

Hello, you might have figured is out by now but you can create objects that change in sizes by using the Change Parameters in the Modify drop down. Look up Parametric Modeling in fusion on YouTube, the videos do a good job explaining it. We have set up Parametric Modeling for our custom door sizes.

I do not have any experience with Alphacam unfortunately, I have only tried fusion and so far it is great.

[alexeletel]

Hello! I was having a difficult time figuring out how to use the ISO file when doing a full 5 axis program so I called a Felder tech and he explained it to me. When you post a program with an ISO file always make sure you create a new folder for it to be saved in. In that folder you will have your .tcn program and a disc file. Open the .tcn file in TpaCAD and click on ISO File on the left. Find your ISO file (the disc image) and click Ok. Optimize the file then open the .tcn file in Cnc Board and run the program. Note: Most collision warnings do not work when using an ISO program so make sure you take it slow the first time running a new program. Hope this helps!

21

[Anonymous]

Glad to see I'm not the only one having issues with this post.  I have 3 issues I need resolved if I'm going to use Fusion 360 as a replacement for my current solidworks/alphacam setup.

1. When I use a swarf command, the iso files' Z zero are at the material bottom.  (Even though the origin is clearly at the top of the material in Fusion manufacturing set up).  This would be no big deal because I could just offset it at the machine, but when I have a 2D contour or 2D adaptive clearing my Z zero is on the top of the material.  I need these two to be consistent.  I'd prefer for the Z-zero to be at the top of the material.  Is there a way to change that in the post?

2. When an iso file is created, the file names are outputted as 0.iso, 1.iso, 2.iso, 3.iso etc.  So when I look at them at the machine in explorer,  I can't differentiate them from one file/setup/partnumber to the next.  Is it possible to get the file name associated with the tcn file to be in the iso name as well?  Example:  "filename.tcn", "filename01.iso", "filename02.iso", "filename 03.iso" etc...?  That way I wouldn't get confused between two different part numbers, which ties into question 3

3. Lastly, I don't understand why WDflash can't look for the iso files in the same location as the tcn file.  I currently have to drag and drop the iso files into Prod/sub because that's where WDFlash goes and looks for it.  It becomes a dumping ground for every 5 axis program with absolutely no revision control.  If I make a change to the tcn file, and 5 more iso's get created, it requires the operator to go find the original 5 iso files and copy over them.  (Its a very uncontrolled system/method and I'd like to fix it.

[josefloresb · Accepted solution]

Hello everyone,

I've been doing many experiments with the post, this is my final version.

It fixes a couple of things:

1. I changed the decimals to 2 because I was having issues if it had more than that for mm.

2. I removed the decimals for rapid movements because sometimes it would jump diagonally from the endpoint of one path and go directly to the startpoint of the next path instead of going up in Z and then moving to the next path. 

3. It fixes the Z value for iso files, now everything is at the correct level.

4. If you tried to machine something that was not in the 1,3,4,5 or 6th face it would create a working plane, but the TPA software was not interpreting this correctly. I changed the Post so now it outputs an ISO file for this cases. The problem is that the angles for the A and C axis are incorrect (I'm still working on that) so the workaround is to create a very simple swarf that has the same angle you need, and then manually copy and paste the A and C angle of this swarf ISO to the other ISO you want.

5. I changed the circular movements to tiny straight lines because sometimes the TPA software wouldn't interpret them correctly, specially for helical movements.

Use it with caution because I am no expert. I just experimented a lot with the PP and so far this version has been working out quite well.

Hope it works for you too.

Good luck,

Jose

[Anonymous]

Hey @josefloresb Jose,

Thanks for your updated post.  It fixed my Z issue, which is a game changer.  Thanks again!

Any chance you know how to change the file name output of the iso files?  See my issue below:

2. When an iso file is created, the file names are outputted as 0.iso, 1.iso, 2.iso, 3.iso etc.  So when I look at them at the machine in explorer,  I can't differentiate them from one file/setup/partnumber to the next.  Is it possible to get the file name associated with the tcn file to be in the iso name as well?  Example:  "filename.tcn", "filename01.iso", "filename02.iso", "filename 03.iso" etc...?   

I continually forget to drag the iso file into Program/sub file in woodflash so I often run whatever previous 0.iso, 1.iso that was previously there.  This is a receipt for disaster and will surly cause communication problems between the programmer and operator.  Thanks again for your help...

Tom

[thomasADXFW]

Hello I can't find any post processor for Felder, where did you found that? Thanks!

[alexeletel]

Hey Thomas,

In the manufacturing tab>manage>post library>scroll down to Felder Profit>then copy it to your local. Hope that helps

[thomasADXFW]

Yes, this help very much thank you. I was confused with machine, not post processor. Felder have no Machine in Fusion. Do you use a generic Autodesk then?