Hello Guest it is August 12, 2020, 02:44:35 PM

Author Topic: newb questions  (Read 4224 times)

0 Members and 1 Guest are viewing this topic.

newb questions
« on: January 14, 2010, 09:47:05 AM »
Hello,
I have built a Solsylva 48x48 CNC mill. i am running it with mach3 and CamBam. This is the first time I have done anything with CNC but I am getting things figured out.

my reason for building the mill is to cut out RC Airplane kits of planes me and some friends have designed.

My question 1:
Is there anyway in eather CamBam or mach3 to bevel the leading and trailing edges of my wings or will I need to get the parts drawn in 3D?

I would like to figure out some way to get the beveling done with my straight bit or a ball end bit. its EPP foam that I will be cutting out of.  the bevels I want to accomplish are like 3/16" down and 1" back on the leading edge of the wing and about the same on the trailing edge.

Question 2:
right now what I have figured out in CamBam for generating tool path cut depths is- i set the final depth inc to .188 for 3/16" foam, my stock surface to 0" and my cut depth to .188". I then zero out to the top of the table and it cuts fine. Am I setting this correct? Is there a better way? I would prefer to zero out Z on the top of the material not on the table top.

Thanks for any and all help

Jon
Re: newb questions
« Reply #1 on: January 14, 2010, 11:00:19 AM »
Jon,

Your 'edges' can be accomplished with form cutters similar to router type cutters. These could be fabricated - either brazed tool steel or clamped pieces ground to the taper required. Then you are making simple straight or even curved edges in 2D. Foam is easy but you may shoot for hardened tool steel cutters so you may cut balsa as well. Balsa is abrasive to cutters. If you don't use form cutters, the only other way is to make the program yourself to do the step-downs in Z or - get into 3D CAM.

Your zeroing is accomplished as you write the program - meaning: if you zero to the top of the material (usual method) then your program will go negative in Z to cut the part. Usually in cutting foam, you would attach the foam to either another piece of foam with double sticky tape or to some other sacrificial table top or surface. That is for two purposes - save cutters and the table and to allow positioning the actual material with conventional clamping arrangements. But, you would zero to the top of the material to be cut and cut going Z negative.

Happy flying...

Bill C.
« Last Edit: January 14, 2010, 11:06:32 AM by BClemens »
Re: newb questions
« Reply #2 on: January 14, 2010, 12:12:36 PM »
thanks Bill
I had hoped to find a different way than a cutter, I have found one that would do the angles I want but then there's an extra bit change and extra material loss, also my parts have to be further apart on the sheet to accommodate the larger bit.

as far as cut settings, Let me make sure I understand, I would set my sheet surface as zero, and my cut depth to -.188? just make my cut depths as neg numbers and leave my surface as 0?

whats the final depth inc setting for? do I leave it at zero? I have tried and I know CamBam wont let me set a neg number for that.

thanks again

Jon
Re: newb questions
« Reply #3 on: January 14, 2010, 12:29:53 PM »
Jon,

You can make up the program to do the tapers with a ball end mill by deducting the sine of the taper from the step-over appropriate for the size ball and part width.... but only in straight longitudinal lines or straight leading or trailing edges. That would work....just a bit of initial figuring then transposing over into a program.

You can do the Zero setting any way you wish. There is no real hard and fast rule for where it should be so that you could use the table at one end/edge of the material or what may make the most sense to you. Sounds like CABBAM just may be making that choice for you anyhow so work with it. There is nothing wrong with the way you are doing it.

Depending on the size of the ball, you may need to take the cutter into the negative Z for these tapers - keep that in mind. The tool (ball) is referenced from the center tip.

Bill C.

Offline ger21

*
  • *
  •  6,282 6,282
    • View Profile
    • The CNC Woodworker
Re: newb questions
« Reply #4 on: January 14, 2010, 12:31:12 PM »

My question 1:
Is there anyway in either CamBam or mach3 to bevel the leading and trailing edges of my wings or will I need to get the parts drawn in 3D?

I would like to figure out some way to get the beveling done with my straight bit or a ball end bit. its EPP foam that I will be cutting out of.  the bevels I want to accomplish are like 3/16" down and 1" back on the leading edge of the wing and about the same on the trailing edge.


I don't use CAMBAM, but I cut a lot of profiles without doing 3D models. I draw a side view of the profile in a CAD program, and calculate where the toolpaths need to be with the ballnose bit I'll be using.

Here's how I do it in AutoCAD.
http://www.cnczone.com/forums/showpost.php?p=681370&postcount=198
http://www.cnczone.com/forums/showpost.php?p=681375&postcount=199

I've done this along curves as well, by offsetting the arcs by the stepover amount, and moving the offset arcs to the appropriate depth.
« Last Edit: January 14, 2010, 12:33:05 PM by ger21 »
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: newb questions
« Reply #5 on: January 14, 2010, 12:37:08 PM »
There you go Jon...!
Re: newb questions
« Reply #6 on: January 14, 2010, 12:48:12 PM »
Wow thanks a bunch. lots of great info there. I will have to try that and see what I can get.
that helps me alot.

Jon

Offline Jeff_Birt

*
  •  1,107 1,107
    • View Profile
    • Soigeneris
Re: newb questions
« Reply #7 on: January 14, 2010, 05:28:52 PM »
>whats the final depth inc setting for? do I leave it at zero? I have tried and I know CamBam wont let me set a neg number for that.

'Final Depth Increment' is a setting in a CamBam MOP that lets you control how deep the last pass is no matter what your depth per pass is set to. This gives you the ability to take the last 0.010" (or whatever) off as a last cut to leave a better finish.
Happy machining , Jeff Birt
 
Re: newb questions
« Reply #8 on: January 15, 2010, 06:00:29 PM »
Jon, over at www.Phlatforum.com, we use Mach3 for running our PhlatPrinters, and Google Sketchup for generating the drawings for our RC models.  Some of the guys there are programmers and have created a plugin called the PhlatScript, for use with Google Sketchup.  (Both the program and the plugin are free.)  The Phlatscript plugin has the ability to designate features as "centerlines" and "fold lines" which will create the gcode for a partial-depth cut along that line.  Using a ball-end or rounded bit, some of the guys have been drawing multiple lines at 1/2 of the bit diameter offset from each other, then cutting the first one at 25%, the second one at 50% and the third one at 75" depth.  The result is a bevel, with very slight scalloping.  The Phlatscript also allows us to designate "Inside" or "Outside" cuts, to maintain climb cuts on the finished surface, place "Tabs" so the cut part doesn't break free of the parent material, and other stuff.
Maybe you should check it out.