Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Best Ways to Reduce Program Size?


parallax7761@comcast.net
 Share

Recommended Posts

Hi Everybody, What do you think the best way to reduce program size on optirough and optirest programs? As you all are aware they can have huge amounts of code and I have a few machines that only have 1MB of memory....Every now and then I don't realize something is going to run on these small memory machines and all the sudden I'm scrambling to chop programs up or reduce overall resolution on the arc filter settings to shrink them. Please let me know what your ideal Arc filter Settings are or any other methods that work well.

Link to comment
Share on other sites

yes it will run "FNC" as they call it on Haas controllers. but the operator doesn't have as much control when running FNC. If I recall I don't think they have override control or something like that. So I chopped it up into 4 programs that would load, that way the operator has control as he proves it out. After we have it proven he is just going to run the whole thing FNC. But I would still like to know the best ways to reduce program size on Dynamic Opti programs.

Link to comment
Share on other sites

Not a real good way to reduce something that by its very nature makes large programs. The whole idea about HST is the in and out and smaller Radial step over. Yes bigger depth, but not sure that is enough to over come the radial difference. I use 50/50 a majority of the time, but if I need to really get small I then kick it up[ to 95/5 and use a loser tolerance. I am roughing within .2 then I might use .02 tolerance. You are roughing within .02 then need to the tolerance and need to code. I broke up one program into 48 tapes for a customer who has a machine with a 2mb limit. I had to think about each tape and check it's size. The other thing is strip out block numbers and comments. 

  • Thanks 1
Link to comment
Share on other sites

First option, as others have mentioned, is to use the Toolpath Filter Settings, to reduce the size of the generated code, as much as possible, before having to worry about chopping up the programs.

Set your "Total Tolerance" to 20% of your "Stock to Leave" value. Say you are leaving 0.04" of material for roughing. Try using these values:

  • Total Tolerance = 0.004
  • Cut Tolerance = 50% (0.002)
  • Filter Tolerance = 50% (0.002)
  • Arc Filtering "on"
  • Check all three Planes (G17, G19, G18)
  • Enable the Checkbox for "3D Arc output"

 

Opti-Rough Filter Settings.PNG

Also, if your single Mastercam Toolpath is just "too big", after being filtered, I would suggest that you use the "Section NCI" C-Hook, to break the single path up into smaller "programs".

Section NCI will break the program into chunks (you specify the max. size), and it adds "retract and approach" moves, for each toolpath section. (Also includes all the Tool Startup, Work Offset, Etc.)

  • Thanks 1
  • Like 3
Link to comment
Share on other sites

Depending on the year (Vintage) of your Haas machine, there is also an option to run a program directly off a USB Drive. This option makes your available program storage much larger. (I seem to remember 8 Gb being the limit for the Haas NGC Controls.)

Running from the USB is just like running from Memory, so all the regular control functions (Feed/Spindle Override, Single Block, Block Delete, etc.) will work off the USB drive. The only real "danger" is if someone happens to unmount the USB drive, while the machine is executing the program.

  • Like 2
Link to comment
Share on other sites
On 10/16/2020 at 8:12 AM, gcode said:

and spaces

Some posts, will post G01 instead of G1,etc.. I think you can strip those as well.

Pardon me for hijacking the thread. Yet, I have seen a lot of scraped parts and machine crashes on some of our older machines when filtering is used. In fact, I had to set "Present arcs as line segments" on "High Speed Toolpaths" . Control definition is set correctly.  I'm thinking that Arc tolerances in the machine parameters for imperial units are set incorrect.

I have read a lot about this issue, yet it's still not clear. Can someone shed some light here?

Thank You.

 

 

 

 

 

 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...