Mastercam Mill 9.1

Discussion in 'Software and Programming' started by azroyhelmy, Jul 23, 2012.

  1. Jul 23, 2012 #1

    azroyhelmy

    azroyhelmy

    azroyhelmy

    Member

    Joined:
    Mar 29, 2011
    Messages:
    16
    Likes Received:
    0
    Hi guys,
    I quite new to the CAM. I'm using 3 axis Fanuc controller mill and 9.1 version of mastercam.

    My question is, how can i control my cutter wear? e.g : I'm ramping a 1" hole to 0.5" depth. my finishing cutter should make the last cut of 1" diameter at 0.5" depth. after checking the hole, the diameter is small of 0.0039".

    So how can i used the 'wear' in tool offset controller? i tried before but the controller triggered an alarm not to do that. should i change the program? If so can anybody direct me to which i should select my 'offset' in Mastercam ?

    Tq
     
  2. Jul 23, 2012 #2

    mulac321

    mulac321

    mulac321

    Active Member

    Joined:
    Apr 26, 2011
    Messages:
    28
    Likes Received:
    2
    Hi there are a few cnc experts on this forum but the best place for thousands of experts is the cnczone.com forum. I believe they have a dedicated section just for master am.
    Calum
     
  3. Jul 23, 2012 #3

    azroyhelmy

    azroyhelmy

    azroyhelmy

    Member

    Joined:
    Mar 29, 2011
    Messages:
    16
    Likes Received:
    0
    thanks Calum
     
  4. Jul 23, 2012 #4

    kvom

    kvom

    kvom

    Administrator Staff Member Administrator Moderator

    Joined:
    Jun 4, 2008
    Messages:
    3,083
    Likes Received:
    583
    You could adjust the tool diameter in MC and regenerate the g-code.

    The best source for info on Fanuc controller issues, IMO, is to register on Practical Machinist and ask your question. Be sure to specify the exact controller model.
     
  5. Jul 23, 2012 #5

    idahoan

    idahoan

    idahoan

    Well-Known Member

    Joined:
    Oct 8, 2008
    Messages:
    557
    Likes Received:
    180
    Tq

    I'm running a rewer version of Mastercam (X5) and in the cut parameters dialog there is box for stock to leave on walls and one for stock to leave on floors. these can be set to a plus or minus value; so in your case you would enter -.002 as this value would only be for the radius. I'm not sure about the older version; but it may have somtining like this.

    I assume that you are using a roughing and then finishing cutter?

    Dave
     
  6. Jul 25, 2012 #6

    azroyhelmy

    azroyhelmy

    azroyhelmy

    Member

    Joined:
    Mar 29, 2011
    Messages:
    16
    Likes Received:
    0
    Yes Dave, I running on different roughing and finishing cutter. Yes, there are dialog boxes for leave stock allowance in mastercam. but , we just don't know the cutter wear, spindle run out and etc that affect the final dimension. so it's quite hard to redraw and repost again to the controller.

    I'm running cnc lathe too, and it's more convenient as all tools offset can be adjust freely.
     
  7. Jul 25, 2012 #7

    Aquaman

    Aquaman

    Aquaman

    New Member

    Joined:
    Nov 5, 2010
    Messages:
    3
    Likes Received:
    2
    There's a box... "Compensation type" I think it defaults to "Computer" click it and you'll see "Control"...."Wear"....etc.

    You want to use "Wear" and re-generate the path. Post it and see if it outputs G42 and/or G43.

    If your post is working correctly and it outputs the codes you should now be able to use the offsets on the control to make tool diameter offset changes.

    Play with it a little on a scrap part.
     
    azroyhelmy likes this.
  8. Jul 30, 2012 #8

    azroyhelmy

    azroyhelmy

    azroyhelmy

    Member

    Joined:
    Mar 29, 2011
    Messages:
    16
    Likes Received:
    0
    Thanks Aquaman, I believe I get it. But when it come to ramping a hole, the controller still not allowed any value in 'wear' column of the controller offset.
     
  9. Jul 30, 2012 #9

    Aquaman

    Aquaman

    Aquaman

    New Member

    Joined:
    Nov 5, 2010
    Messages:
    3
    Likes Received:
    2
    See if you can figure out what "options" are turned on in your control.

    In my experience, the controls come built with all the options included and the re-seller turns on those options that you pay extra for....
    If something called "Helical or Tornado" isn't turned on in the control its probably not going to work and you'll have to use Circle Mill or the regular contour path in order to use your control offsets.

    Try clicking "Compensation type" and "Control" and re-gen your path and post it.

    You just have to fool with it until you get the machine to do what you want.

    An easy way to size the hole is to just draw another circle that's .0039" larger than the one you just cut and drive the tool on the new circle as the finish path.

    Whatever gets the hole to the size you want it to be......;)
     
  10. Jul 30, 2012 #10

    atheras29

    atheras29

    atheras29

    Member

    Joined:
    Apr 27, 2011
    Messages:
    18
    Likes Received:
    0
    Hi
    Post from Master Cam the existing post again and before sent it to mill change the diameter of the existing # tool under description of tool

    ( make it smaller off .0039'')

    second line under the first G codes

    if you have any problems please post a picture of the post to help you

    good luck
     
  11. Aug 14, 2012 #11

    Justin_Sane

    Justin_Sane

    Justin_Sane

    Member

    Joined:
    Aug 14, 2012
    Messages:
    5
    Likes Received:
    1
    This is a bandaid fix. not proper method. You should add an entry motion. Your controller is throwing an alarm because you cannot start a cutter comp on an arc motion. it must lead in straight to activate the cutter comp and arc after its active.

    Also use wear comp, and do not use any geometry (radius) in the control when setting up. Ie you should set the tool length only, no radius. Then use your wear comp value to adjust the .0039".

    It's been a long time since I used/trained mc9 so I cant tell you where the exact commands are, but you should have lead in lead out options, use start at centre and perpendicular entry. I have MCX6 currently.
     
  12. Aug 14, 2012 #12

    kvom

    kvom

    kvom

    Administrator Staff Member Administrator Moderator

    Joined:
    Jun 4, 2008
    Messages:
    3,083
    Likes Received:
    583
    WRT not using the radius in the control: I believe this means you tell MC to offset the toolpath rather than the control, so define the tool in MC.
     
  13. Aug 14, 2012 #13

    Justin_Sane

    Justin_Sane

    Justin_Sane

    Member

    Joined:
    Aug 14, 2012
    Messages:
    5
    Likes Received:
    1
    The way mastercam outputs the toolpaths with the comp options is basically this,

    -computer (no comp command, coordinates are tool centreline)
    -wear (comp command g41/42, coordinates are also tool centreline, but tool shifts to the proper side by the amount of wear comp in control, usually a very small number), leave the geometry (rad/diameter) column to zero on the control of the machine)
    - control (comp command g41/42, outputs coordinates of the geometry, this is used when you are entering the tool radius or diameter (depending on control settings of machine) into the tool geometry, this allows you to change the tool from say 3/4" to 1/2" at the control rather than by changing the toolpath. this can cause issues though if you allow the operator to decide what tool diameter to use. This can also use the wear comp on the machine to make minor adjustments with this method.

    You can tell mastercam that the tool is a smaller size to adjust the toolpath with comp set to computer, however the next time you run it with a brand new tool, you might overcut your part.

    use wear comp with a lead in motion on the helix and you can make minor adjustments while still retaining the proper programmed coordinates. That is pretty much the industry standard way. Most of my customers use it that way anyways :)

    also one of the previous comments suggested that an option may not be available. That would not matter as you can easily output point to point code that will do the same thing. all the helical or tornado option is, is a macro canned cycle that does the cycle with a one line call. Very nice for when you want to punch a quick hand program on the control, but not necessary when using a CAM system.
     

Share This Page