Author Topic: Other Post Processors - But Not Directly About CamBam  (Read 1268 times)

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3913
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Other Post Processors - But Not Directly About CamBam
« on: January 19, 2018, 15:47:03 pm »
I recently have been fighting with some steel press dies.  Small details.  Difficult machining.  I've been working on it for weeks.  One of the other members here did the 3D work for me.  He's very good at it.  I paid him for the work, and feel it was worth every penny.  You are welcome to plug yourself if you like, but please do not post the images. 

Anyway, I tackled the smallest ones first and CamBam kind of choked on it.  There are three main issues. 

1.  CB does not do any kind of HSM or constant engagement strategies in 3D.  I broke a few hundred dollars worth of cutters trying to get something that would work.  Not to worry.  Its a hard material.  I planned for that, but after days (weeks) of trying I felt I was getting nowhere.  My only success was to use speeds and feeds that were calculated based on 100% engagement at full depth.  It sort of worked for roughing.  Ultimately the job would have taken about 9.5 hrs for the fastest die.  I tried it anyway.  I still broke cutters on finish passes. 

2.  Boundary limitations are inside boundary only.  Ok, a negative boundary margin of the cutter radius sort of works, but the tool path does not seem to actually account properly for being able to cut at the contact point.  Only at the tip and only if there is clearance.  Not if there is clearance for the diameter of the tool at THAT depth.  I could have played with it some more, but I butted up against so many other problems I didn't have the time to spend with it.  I have used plane slice only to overcut parts before, but this would not have worked here. 

3.  There is no real rest machining operation.  None at all.  This meant with CamBam every successive operations had to be treated like 100% engagement at full depth, and since CB doesn't differentiate between vertical and horizontal in 3D this meant operations that were mostly a skim cut still had to be set for speeds to match full depth at 100% engagement to prevent breaking a cutter every time it came to a corner. 

This lead me to look at Fusion360 again.  Its not perfect.  I ran into plenty of issues.  Not the least of which is that REST is not 100% perfect, and its only available with some types of operations.  Ultimately I had to accept that I could not machine with the smallest cutter I wanted to use for my finish pass.  I never came up with a strategy that didn't break it repeatedly.  It might be runout.  It might be machining tool paths.  It might simply be a limitation of the fact that the material can work harden, and the finish pass with the smallest cutter wasn't going through the work hardened area of the previous operation. 

Anyway... this brings me to my point.  The default Mach3 post processor. It inserts extra code.  Specifically it inserts optional stops and tool change position moves (M1 and G28) at the end and beginning of operations respectively.  This could be both a help and a hinderance to beginners.  An optional stop seems like it might be ok, but sometimes it seems to prevent operator input and Mach3 can already be set to stop when it receives a tool change command.  Its sort of redundant.  You have to press start to get to the tool change command.  Then the G28 takes it to the tool change position, which I no longer use.  I actually use G53 moves in my tool change macro.  Its only a minor inconvenience since my G28 position has been set to something safe on all my machines, but if I recall it was not set to anything useful when I first started CNC machining.  It could confuse the heck out of a new user.  Maybe its safer sometimes, but if safe Z moves is not turned on and a safe z height set you could have a crash caused by this. 

I actually use the default Mach3 Post processor exactly as it comes from CamBam.  My machines are setup so they control their own safe moves for tool changes, and they account for the fact that by default doesn't put out all axis coordinates after a tool change by saving the current position as part of my tool change macros.  I felt like I had to modify the Mach3 post processor from Fusion360 right out of the gate.  Worse, when I installed Fusion on a new computer my modified post was not installed with it even though Fusion is supposedly a cloud based application. 

Be aware if you use it for collaboration that the person working with you is NOT using the same post as you are.  Its ok if they have it setup to be cut on their machine, and you have it setup to be cut on your machines, AND you only run your own code.  If they send you code it may be no good.  I really like to try to setup my machines so that except for feeds and speeds capability all the code is cross compatible.  At this point that is true for my machines.  The last thing I need is another level of confusion. 

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2296
    • View Profile
Re: Other Post Processors - But Not Directly About CamBam
« Reply #1 on: January 20, 2018, 13:00:48 pm »
I may be wrong but IMO CamBam has internally the methods and functions which can form more complex and flexible 3D MOPs.
I see many people had read the thread but no comments added. It would be interesting to see a discussion here and experience shared by others. Both about usage of CamBam and comparison to other programs/methods.