Author Topic: Gcode Request for a part  (Read 11498 times)

0 Members and 1 Guest are viewing this topic.

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #10 on: August 20, 2015, 02:39:57 PM »
Here is a link to the actual presentation where you can download and run it. You can rotate, speed/slow etc just as you could if in BobCAD itself..

http://WDMyCloud.device2441142.wd2go.com:9093/api/1.0/rest/file_contents/Public/N54%20Charge%20Pipe%20Adapter.exe?device_user_id=15760889&request_auth_code=c291222ed591f12b51ceec6d9d5602a919e768dbaa832148abd37e838cff06a2



Hood

Offline lcvette

  • Active Member
  • Posts: 62
    • View Profile
Re: Gcode Request for a part
« Reply #11 on: August 20, 2015, 02:47:59 PM »
Hood,

Saw the video, looks awesome! my simulation looks pretty much identical so it should make it as accurate as possible.  mach accepted it and ran it same as simulation so i know i have a viable starting point of how the code should look, now just need to go through all of the settings in the UPG and keep tinkering with them until they spit out the appropriate code.  You are the friggin man and I can't tell you how much I appreciate your help on this!  I wrestled the same thing while  straightening out the post for the mill, but eventually got it working flawlessly.  Unfortunately I know infinitely less about lathes and lathe code so it is a bit of a learning curve.  I am making models of all of my tool holders and inserts so it has accurate geometry to use in it tool path generation, unfortunately it doesn't have anything preloaded for tiny tools like I am using..lol

I will work on it some more tonight when i get home and see if i can make heads or tails of anything!  Again, thank you so very much for your help!

Best Regards!

Chris

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #12 on: August 20, 2015, 02:53:09 PM »
What CAM are you making the post for, is it LazyTurn?

You can often download DXF or IGES files from the likes of Sandvik or Seco or Kenametal for your tools.
Hood

Offline lcvette

  • Active Member
  • Posts: 62
    • View Profile
Re: Gcode Request for a part
« Reply #13 on: August 20, 2015, 02:54:32 PM »
that is great information, hadn't though if that!  I'm using Camworks.

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #14 on: August 20, 2015, 02:58:17 PM »
Ah ok, never used that.
Hood

Offline lcvette

  • Active Member
  • Posts: 62
    • View Profile
(No subject)
« Reply #15 on: August 23, 2015, 12:30:07 PM »
I've got it outputting useable code, everything looks good with the movements, just trying to write a decent tool change command.  It has a few different areas to configure such as rapid to tool change, initial tool change, subsequent tool changes and rapid from tool change.

Alot of it is confusing because it will stop for a tool change with different codes and not necessarily an M6.

And of course it is alot of trial and error with the language and how to format it properly.  All in all I love the fact it allows me to make changes and I know I will get it there, just going to take a little tinkering on it.

What I have learned is how little I know about lathes verse milling machines.. I wrestled with code being wrong for 2 days before realizing that a rear turret is a traditional turret on a lathe, once I figured that out everything started jiving with the actual movement code.

I noticed you use an M7, any reason for that over an M6?

Being I am using a G0704 mill with the head turned 90 degrees, I don't have home or limit switches setup for the lathe so determining where to send the lathe for tool changes is odd.  Between having some control in the cam software for safe retracts and indexing positions I am wondering if I would just be better off using the cam to send the mill to a tool change position and just use the post to call for the M5, M9, and M6 and subsequent G97, M3, S word, M8..

Also when zeroing a part on a lathe I always did so at the outer edge of the stock diameter and face.  Am I to understand correctly that the tool offsets to the center handle everything else?  Haven't added a tool library yet.

I assume that the tool offsets will be handled in mach3 so I have then turned off in the cam software.  However for the tool tip, in the cam I have to set all of the tools up by the center point of the tool tip radius and set it as the 0, 0, 0 coordinate in the model.  Will this conflict with the mach tool table settings?  I am unclear if the gcode is posted with the tool tip radius taken into consideration and if so which would be the better solution to make the tool tip a point in the cam and let mach3 handle it or set it to zero in mach3 and let the cam handle it.

Any thoughts?

Sent from my XT1080 using Tapatalk

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #16 on: August 23, 2015, 06:11:51 PM »
M7 is my coolant, I used to have a front and a rear turret so I used M7 for my rear turrets coolant and M8 for the front turret.

 M6 is for a tool change but on Mach Lathe it is not required, You can use M6 if you wish or not if you don't, I choose not to, all you need is the T****.

X0 is the centre line of the lathe, so if you take a skim cut and measure the diameter (assuming in Dia mode) then you enter that value in the tool table.
Here is a vid I did showing how to set up some tools which may help.
https://www.youtube.com/watch?v=mWnfioI3G0E

You can change a tool at any position on a lathe, often you code it so that the tool is just clear enough to not hit anything.
Hood


Offline lcvette

  • Active Member
  • Posts: 62
    • View Profile
Re: Gcode Request for a part
« Reply #17 on: August 24, 2015, 12:05:03 AM »
Hood,

Thanks a million!  very informative and very helpful.  I went ahead and used the M06 call in the post because I have machstdmill/lathe and will likely use it down the road so it is nice to have all the buttons in places that are familiar..  i have not dug into it yet, but i believe it uses a tool change macro which can be setup similar to the mill profile.  for now i just used a safe retract function in the cam software that will automatically remove the tool and send it to a designated indexing position at a tool change call, currently setup for x2 z4, I will probably change the x to 2.5", i have a 4" lathe chuck and my mastertool is the longest tool in my box so it should always give me clearance for any changes i need to make, and without a tail stock, i doubt i will be turning anything over 4" long so should be good there as well.

I attached a copy of my post, I will be using a cored 2" piece of stock for these parts and I haven't yet added a cutoff tool to generate that toolpath yet, probably tomorrow.  the only tool i had was a neutral 35* diamond insert to cut the back portion of the part which is why it is creating a V.  You got me all hot and bothered about a round insert and tool holder but i haven't found any budget oriented offering for one yet, i could see that tool being VERY useful!

I really appreciate all your help, I am currently cross eyed from going through the post code, very intimidating for someone who has never programmed anything before.. just shear will was driving me on..hahaha

let me know what you think of the code, a few things that were killing me was that everytime i would put a G91.1 in the post it made things screwy.. so i ended up just setting the post to have all I,J moves output in incremental and with mach set for I, J moves to be incremental it seems to jive just fine.  i have the feed setup to call for either fpr or fpm depending on what i click in camworks, being i am unfamiliar thus far with values set in fpr and have gotten some experience from manual jog turning and using the wizards for basic turning jobs, i will probably stick with them for a while until i feel good about everything else.

you da man!

Chris

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #18 on: August 24, 2015, 06:12:35 AM »
Did you attach the correct code? Looks like the file I attached. The .set one just seems to have the tool designations in it and noting much else. maybe it needs the CAM to open correctly? I was just using Notepad++

Regarding the feed,  much better to use G95 on a lathe  in my opinion as you will normally only use a few different feeds. For example on my big lathe I tend to use 0.25 to 0.3mm per rev for roughing and 0.15mm per rev for finishing. Altering the spindle speed for different materials and diameters will not affect the chipload. If using Feed per minute then you will have to enter different values depending on the RPM to try and keep the chipload constant.

I have been asked a lot of times when I will do the video for tool setting with home switches, I have never got round to doing it. I may not have the wee lathe for much longer and using a camera and setting tools on the big lathe is a bit more tricky, so now  I have home switches on the wee lathe I  better try and do it soon, basically it is a similar procedure but rather than having a master tool you use the home switches as the master.

Regarding tool change position, normally you let the CAM handle that as it is easily changed in CAM and means you do not waste time gong to a designated position if it is not required to move as far as that.

Hood
« Last Edit: August 24, 2015, 06:24:50 AM by Hood »

Offline Hood

  • Mach4 Alpha
  • Posts: 25,774
  • Carnoustie, Scotland
    • View Profile
Re: Gcode Request for a part
« Reply #19 on: August 24, 2015, 06:22:16 AM »
Oh and regarding the round tool I used in the simulation, it is a Seco MDT which can be used for light turning or grooving and can use 3mm round end inserts as well, quite a handy tool but quite expensive. I was going to get a Korloy MDT tool but I found a good deal on Seco insers so went with that instead.

MDT stands for Multi Direction Turning.

Here in the UK there are places that sell round insert tools for smaller lathes which are fairly cheap, here is a link to one such tool although it is a 6mm insert rather than the 3 that the seco has.
http://www.shop-apt.co.uk/apt-90-srdcn-lathe-turning-tools-for-rcmt-inserts/srdcn-1212-h06-apt-lathe-turning-tool-for-rcmt-0602-inserts.html


here is a link to a video of the Seco MDT tool

https://www.youtube.com/watch?v=cLz-uEvQatI


Hood