Hello Guest it is November 19, 2019, 04:56:32 AM

Author Topic: Gcode Request for a part  (Read 12479 times)

0 Members and 1 Guest are viewing this topic.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #30 on: August 28, 2015, 05:25:10 PM »
Yes, inserts specific for Alu usually have a high positive rake and are also usually ground and polished to give a sharp edge.
Having said that I usually don't bother with special inserts when doing Alu, but the results depend on the type of Alu being cut. Cast alu usually cuts nicely and as I do mainly marine work the alu grades I use cut fairly nice.
 I do not really like cutting Alu on the manual lathe, much prefer stainless :)

Hood
(No subject)
« Reply #31 on: August 28, 2015, 07:43:15 PM »
Stainless?   I tried that on my mill and didn't get hang of it, tried allow, fast, deep cuts to avoid work hardening... Just ended up destroying endmills... Guessing machine rigidity had alot to do with it along with motor power.




Sent from my XT1080 using Tapatalk
(No subject)
« Reply #32 on: August 28, 2015, 08:23:17 PM »
I think I know the answer to the question but I'm not positive and thought it best to ask.  When setting up the offset for a boring bar on the QCT post, do I set it off the back of the work piece?  Or should I use a piece of metal against the the stock and set it against the overhang of the metal off the edge of the stock?  I'm using mach standard mill with master tool mode and got a little confused in this part during the tool offset setup.

Thanks!

Sent from my XT1080 using Tapatalk

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #33 on: August 29, 2015, 03:54:01 AM »
Stainless turns easily, just dont have the RPM too high and keep the feedrate up, it is similar for milling.

Setting boring bars up you can do it several ways.
You can take a cut of an internal diameter and measure.
You can, if you have enough travel, touch off the opposite side and enter a negative value.
You can use a piece of tool steel, or similar, held against the part and bring the tool out on X, you will easily feel as it touches.



Pic below of the last method although it is for the opposite hand of tool than I think you are using so is on the opposite side.
(No subject)
« Reply #34 on: August 29, 2015, 12:45:25 PM »
That appears to be the same tool as the one I have.  I have enough travel to touch off the back no problem, so I will give that a try. 

Sent from my XT1080 using Tapatalk
(No subject)
« Reply #35 on: August 31, 2015, 05:53:18 PM »
Hood,

I'm confused again..lol

I was reading the mach manual and it suggested letting the cam software handle the tool offsets?  Is that correct?

This is easy I'm sure, but I am terrified to crash this thing.  Do you let mach handle the offsets or your cam package?

Thanks!

Chris

Sent from my XT1080 using Tapatalk
Re: Gcode Request for a part
« Reply #36 on: August 31, 2015, 06:56:02 PM »
Ok,  I am glad i got confused because it forced me too look a little deeper and even with my cam package set for CNC Compensation off, it is still accounting for the tool tip radius.  I am using tools with a 1/64 (.015625") radius tip and it is showing the X going to X -0.156 on facing operations.. glad i caught that or it would have been doubled by mach if i entered the tool radius into the tool table.  so I know I can go back in and fix all of the tools I drew for Camworks and set the tool tip radius as a zero point and it will spit out unadulterated code and then have mach handle it, but it seems to me that letting the cam do it may be better?  keeps mach from having to do the calculations?  however, i need to now figure out what else this is going to effect such as part zeroing etc.  it appear there is a gauge offset in the camworks tooling table for both the X and Z in the tooling page.  it wants to set the offsets off of the flat of the square bar portion of the tool holder (the clamped section) for the Z and for the X it wants to offset from the rear edge of the tool.  when i zero them out it shows the offset to be the tool tip radius center point.  I wonder if I need to set the offset so the point shows the tool tip where it would be if there was no radius and the tip came to a point?  thoughts?

Soo confusing!

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #37 on: September 01, 2015, 05:52:55 PM »
I don't know what your CAM calls the compensation but usually you have two types in the CAM.
In BobCAD they call it System Comp and Machine Comp.

System Comp will take into account the nose rad and you can also have collision detection so that it will take into account the shape of the insert (and holder if defined)
I have this turned on.

There is also machine comp where BobCAD will use G41 and G42 outputs  rather than producing a "true" toolpath code.
I have this turned off.

So basically I let the CAM handle the nose rad and collision detection and output the true path.
Mach itself handles the tool X and Z offsets.

Screenshots below showing the various options in BobCAD.

Hood

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #38 on: September 01, 2015, 05:53:59 PM »
And this is the option I use, although occasionally I will use the option of no collision detection (last pic in previous post)

Hood
(No subject)
« Reply #39 on: September 01, 2015, 11:59:22 PM »
Hood,

Excellent, that is exactly how I decided to set Camworks up as well.  It handles tool paths based on the tool models I designed and the zero point being the center of the tool tip nose radius so it is outputting true tool paths and I do the the X and Z offsets in mach3.  I have a part chucked up and am just tweaking the tool paths bit plan on hitting the go button tomorrow. 

I had been wrestling with the post trying to change the feed option between ipm and fpr and was stumped because the post template I was using, (fanuc generic) called for g98 or g99. finally out of the blue I saw a small check box on the fanuc source code in the universal post generator that asked if I wanted post style A, B, or C. Apparently B and C output that command as G94 and G95 which was what mach needs...  So now I'm in business and think the post is 100% mach compatible at least for anything I have test posted so far..lol

So thanks so much hood for the confirmation!  It also allowed me to run the same safety line up top without tripping error codes!

Double bonus!

Chris

Sent from my XT1080 using Tapatalk