554,275 active members*
3,535 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Rhinocam > Rhinocam - tolerance to account for machine actual cutting size
Page 1 of 2 12
Results 1 to 20 of 21
  1. #1
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Rhinocam - tolerance to account for machine actual cutting size

    I have the following challenge.
    I need to cut a 0.25" hole for some metal pins. However my machine is cutting this feature a little small at 0.245 and therefore the pin will not fit.
    The tolerance is for the operation I am using is set at 0.001 and the circle for the hole is drawn at 0.25.

    Other than drawing the circle a little bigger to account for my machines inaccuracy, (which is what I ended up doing) is there a way in the software to manage tackle this challenge. I know aspire has a way to cut slightly larger or smaller.

    I appreciate the feedback.

  2. #2
    Registered
    Join Date
    Aug 2010
    Posts
    599
    Yes just set your stock material using + or - numbers to adjust how much over or under to cut. The box under tolerance. Also might want to do a spring pass to make sure it isn't simply endmill deflection.
    warmachinellc.com

  3. #3
    Member
    Join Date
    Apr 2004
    Posts
    5539

    Re: Rhinocam - tolerance to account for machine actual cutting size

    You might think about leaving it slightly undersized and using a reamer for the final few thousandths. It's hard for a machine to make a perfectly round circle by traveling around it on the inside with a smaller tool. But yes, like Swath says, try going around another time or two to see if the tool cuts a little more then.
    Andrew Werby
    Website

  4. #4
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    Quote Originally Posted by SWATH View Post
    Yes just set your stock material using + or - numbers to adjust how much over or under to cut....
    But correct me if I am wrong, the tolerance values basically control how much material to leave (extra) as opposed to how much extra to take out.
    In other words, unlike aspire, in rhinocam you can only go - xx.xx and not +/- xx.xx. You can only go in one direction (unless I am missing something) and that is what I am asking.

    So in the example of the hole, if I draw it at 0.25" and the machine cuts it at 0.24" my solution has been to draw the circle at 0.26" so that my machine cuts it at the correct size.
    if I were to use the tolerance parameter and input the value 0.01", the machine will cut a smaller hole = 0.23" in my case. Furthermore, the parameter will not allow my to input -0.01" which I would think would cut the whole bigger.

    Aside from this, What is a spring pass? is it a finish pass?

  5. #5
    Registered
    Join Date
    Aug 2010
    Posts
    599
    Not the tolerance value but the stock value. Adding a positive value leaves more stock than the programmed feature. A negative value cuts more material than the programed feature. I do this all the time to tweak hole sizes without futzing with the model or drawn curves. A spring pass is just another go around a previous cut without any taking any more material. In reality it usually takes a little because one pass with cut slightly off due to endmill deflection.
    warmachinellc.com

  6. #6
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    I see what you mean. I guess unfortunately hole pocketing lacks this feature..
    Take a look.

    it is such a small hole that it would be hard to "profile it."


  7. #7
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    by looking at the screenshot I posted I realized that I could probably use the "Hole Diameter (D)" field and use that compensate. So in my case if I am cutting 0.005 too small for a 0.25" diameter hole, I can type in 0.255" on that parameter and not use the geometry.

  8. #8
    Member
    Join Date
    Jan 2005
    Posts
    14305

    Re: Rhinocam - tolerance to account for machine actual cutting size

    FoxCNC1

    If you are going to do adjustments, it is always better to change the tool size in the software, you also want to set the Tolerance to .0001, one thousandth (.001) is way to big a number for precision holes

    Of cause cutter comp is the best way to adjust for cutter size, with a small hole cutter comp may not be usable though as you have to have at least half the cutter diameter lead in for it to be used
    Mactec54

  9. #9
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    ..yikes over my head i thnk...
    I think you said you make my tool diameter smaller in the software to compensate.
    Now what do you mean about the tolerance? my rhino file is set to .0001 though.

  10. #10
    Member
    Join Date
    Jan 2005
    Posts
    14305

    Re: Rhinocam - tolerance to account for machine actual cutting size

    FoxCNC1

    If it is already set at .0001 than you don't have to change anything

    Yes you can just adjust the tool diameter smaller in your case, to get the right size hole,
    Mactec54

  11. #11
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    You know what the issue with the changing the tool size is? that other features that are cutting properly will now be smaller. And I think this whole challenge had to do with the size of the hole I am making and the "lack" of precision of a cnc router (versus and mill?)

  12. #12
    Member
    Join Date
    Jan 2005
    Posts
    14305

    Re: Rhinocam - tolerance to account for machine actual cutting size

    FoxCNC1

    No because the holes in your case are important, you would run that as a operation by it's self, no other operations would be affected, yes if you are doing this on a router, it would have to be very well built, to be able to hold .001 for a hole, you could use a reamer if you can get the spindle to run slow enough
    Mactec54

  13. #13
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    Quote Originally Posted by mactec54 View Post
    FoxCNC1

    No because the holes in your case are important, you would run that as a operation by it's self, no other operations would be affected, yes if you are doing this on a router, it would have to be very well built, to be able to hold .001 for a hole, you could use a reamer if you can get the spindle to run slow enough
    I think I understand. You were suggesting that I can configure a tool with the allowance or tolerance built in and use it just for that particular operation, for example in my case "Bit for 0.25 holes on plastic". I can then without physically changing the tool, just use a different tool definition for the other operations.

    I also goggled reamer, but I don't think the same tool you are suggesting comes up. What do I need to search by? I keep getting hand held spear like conical tools

  14. #14
    Member
    Join Date
    Jan 2005
    Posts
    14305

    Re: Rhinocam - tolerance to account for machine actual cutting size

    FoxCNC1

    Yes as far as the tool goes, do all operations as a separate op, you can if you want to call the same tool but with a different tool # T3 .245 & tool T2 .250 for your profile

    Reamers come as HSS or Carbide, but if you are cutting plastic, then most of the time, the reamer will cut under size, so you may be better to play with your cutter/tool size to get the size hole you want

    Over & Undersize & Dowel Pin High Speed Steel Straight Flute Chucking Reamers | Travers Tool There are many other suppliers as well

    Bits are for drill holes woodworking/metal working, anything that has Flutes Etc for milling are called by there name Like Endmill Ballmill Etc ( Cutter ) is a good way to describe what you are using
    Mactec54

  15. #15
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    Quote Originally Posted by mactec54 View Post
    FoxCNC1
    Yes as far as the tool goes, do all operations as a separate op, you can if you want to call the same tool but with a different tool # T3 .245 & tool T2 .250 for your profile
    Reamers come as HSS or Carbide, but if you are cutting plastic, then most of the time, the reamer will cut under size, so you may be better to play with your cutter/tool size to get the size hole you want
    Over & Undersize & Dowel Pin High Speed Steel Straight Flute Chucking Reamers | Travers Tool There are many other suppliers as well
    Bits are for drill holes woodworking/metal working, anything that has Flutes Etc for milling are called by there name Like Endmill Ballmill Etc ( Cutter ) is a good way to describe what you are using
    Can you please elaborate why the reamer will cut undersized in plastic as opposed to another material (you didn't say by the way)?
    When you are using a reamer you you need a "real" spindle and not a wood router is what I am gathering since I have to turn it slowly (how slow). I am guess you also programmed it a a drill operation is this correct?

    By the way thank you for pointing out the correct terminologies. I am cutting with a 2 flute endmill.

  16. #16
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    I wanted to tell you guys that your suggestions helped very much. I am now looking at adding counterbores and chamfers to my parts. Not sure how to add those tool paths can someone give me some pointers?

  17. #17
    Member
    Join Date
    Apr 2004
    Posts
    5539

    Re: Rhinocam - tolerance to account for machine actual cutting size

    To do a counterbore, select the hole (either a circle or the point in the middle will work) and use a drilling operation with the appropriate-sized tool set to the depth you want to bore to. To do a chamfer, select the edge you want to modlfy and set up an engraving operation with a V-shaped tool that is lowered to the correct position, which depends on how much you want to take off.
    Andrew Werby
    Website

  18. #18
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    I had asked a friend about this, but I will ask you since you are quite familiar with rhinocam. I usually cut in multiple passes, I did not see a option to do this in Rhinocam when using the specific chamfer toolpath. Is this one of the reason you suggest to use a regular engraving path? I am afraid to run a single pass in aluminum or plexi.

  19. #19
    Member
    Join Date
    Apr 2004
    Posts
    5539

    Re: Rhinocam - tolerance to account for machine actual cutting size

    I tend to use Engraving for everything involving linear cuts, but you can also do it with the special Chamfer settings. The Chamfer operation simplifies things by doing the math for you, so you don't have to calculate the width of your chamfer. It also makes sure you've got enough clearance for the tip of your tool. You're right; it's a good idea to take it easy and go around a few times instead of trying to do the whole thing at once; you'll get a better finish that way. You can set the Chamfer machining operation to do it in multiple steps; there's a Stepover Control panel at the bottom of the dialogue that lets you do that by width of cut or steps per cut.
    Andrew Werby
    Website

  20. #20
    Registered
    Join Date
    Jul 2013
    Posts
    608

    Re: Rhinocam - tolerance to account for machine actual cutting size

    there's a Stepover Control panel at the bottom of the dialogue that lets you do that by width of cut or steps per cut.
    Let me take a look again. I may have missed it.

Page 1 of 2 12

Similar Threads

  1. Virtual CNC machine that takes material type into account
    By monsieurmark in forum Uncategorised CAM Discussion
    Replies: 0
    Last Post: 07-15-2014, 11:59 PM
  2. middle size, up and down table, laser cutting machine
    By vivinar in forum General Laser Engraving / Cutting Machine Discussion
    Replies: 0
    Last Post: 05-18-2012, 09:06 AM
  3. Large size laser cutting machine DC-1324
    By mandyfang2006 in forum News Announcements
    Replies: 0
    Last Post: 01-13-2009, 10:14 AM
  4. Where can I find Good CNC Wood Cutting machine for Car parts size ?
    By Calico in forum DIY CNC Router Table Machines
    Replies: 3
    Last Post: 02-28-2005, 06:36 AM
  5. Do you account for climb cutting in G code?
    By fyffe555 in forum DIY CNC Router Table Machines
    Replies: 12
    Last Post: 11-07-2003, 02:21 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •