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.
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.
Re: Rhinocam - tolerance to account for machine actual cutting size
Quote:
Originally Posted by
SWATH
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?
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."
http://i10.photobucket.com/albums/a1...ps4e18fdc8.jpg
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.
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
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.
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,
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?)
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
Re: Rhinocam - tolerance to account for machine actual cutting size
Quote:
Originally Posted by
mactec54
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
1 Attachment(s)
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
Re: Rhinocam - tolerance to account for machine actual cutting size
Quote:
Originally Posted by
mactec54
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.
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?
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.
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.
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.
Re: Rhinocam - tolerance to account for machine actual cutting size
Quote:
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.