LinkBack URL
About LinkBacks
I was able to fix Bob's post pro. they had a G95 in there for feed's and you could not turn it off in the software .
I will check further today for threading and other function's to see if they will run OK .
| | |
Does anyone use V24 with lathe inch post. I have been trying to get one from bobcad for three months now with no luck.
They sent me one but it will not work either so, i am kind of stuck except for the wizards in mach.
I was able to fix Bob's post pro. they had a G95 in there for feed's and you could not turn it off in the software .
I will check further today for threading and other function's to see if they will run OK .
Hi,
I am trying to get V24 to work with my lathe on Mach 3 and am struggling with post processors. Tried Mach3LathePst and hit a problem with "no S word G96 line 19" - I edited the tool path in Bob to go for a fixed RPM and this seemed to sort that out - I then got a new problem - "F word missing with inverse time arc move line 24"....whatever that means
Have we got a proven post processor for Mach3 that could be shared? I found the older thread on this which didn't seem conclusive. The BobCAD web site has a string of Mach3 turn post porcessors but gives no clues as to which works and indeed why there are more than 1 in the list.
Can Al step in here and help get this sorted??
Thanks
Ian
I would think the standard single line lathe post would work or be a good starting point. I would agree there are many mach 3 posts on the website and god only knows which one is the right one for you, or you or you....
So I am sure we can come up with a solution together. Do you have the single line lathe post? I've attached it. Please post some simple samples and let's get into it.
Also if anyone has a mach lathe post that is known to work, please post it here for us.
Al DePoalo
Partner Product Manager BobCAD CAM, Inc. 866-408-3226 X147
Hi Al,
Thanks for getting back to me on this. I had spoken with support before as the post I had been using was not posting a proper header to get Predator going - The Engine Guy was also very helpful in getting this sorted - you should get him on the payroll along with Burrman!
I attach this post here.
I have continued to work on that little roller thing mentioned in an earlier thread.....it is amazing how much time can get eaten up pursuing these things but it is all part of the learning curve I guess!
Here is the G code (note in radius mode) that BOBCad is generating and Predator is simulating nicely.
Mach is however making a meal of it.....it is as if it is interpreting the arcs "inside out" i.e. rather than follow the path of the bit of the arc BOBCad intends, it goes roun the rest of the circle.
Sure this is a config issue in Bob or the post processor or even Mach - question is which one?
Ian
Just shooting out for the day - but I just wondered if this is to do with he machinie orientation? BOBCad assumes the tool is coming from the back of the job (where it often is in proper CNC lathes) but in reality the tool on my lathe is coming from the front. Does this mean that CW and ACW are reversed? Should we swap G02 for G03?
When I get back later on I will generate some code using the Mach turning wizard then do the same geometry with BOBCad and compare them - should be revealing.
Ian
BobCAD assumes the tool is coming from either the old front approach to the material with the toolpost closest to the operator, this also applies to a "standard" slant bed type lathe that approaches the material from the rear but the tool is facing downwards.Originally Posted by xj5373
This is in effect exactly the same, it is just taking the front toolpost and rotating it around the center line of the lathe so the tool turret/tool post is at the rear.
So, imagine I have an old Lathe with the tool post at the front and using manual tool changing, I wouldn`t change anything from the BobCAD output as BobCAD has already output the code correctly for a rear approach with the tool facing down so that is still correct for my setup.
All the above has the spindle rotating in a standard clockwise direction when viewed from the back of the spindle, not from the chuck, ie M3.
Things only change when you have an "oddball" machine like one of my Lathes, it is a slant bed type with the tool turret at the rear, so far so good, however the turret is setup so the tools are facing upwards which means the spindle has to rotate in the opposite direction ie anti-clockwise so I have to have my Post Processor setup to output an M4 instead of an M3.
One small point, Mach does run in Diameter mode, the numbers on the screen are the diameter of the workpiece so it is entirely possible that it doesn`t like the code arcs you are giving it.
As you can see and from the above and what Al posted there is no "post that works for every one" the post has to be "tweaked" to suit the machine/operator as due to the ability to setup Mach to work differently for different machines/operators.
You haven`t given us much in the way of details of the physical characteristics of your Lathe which makes it difficult to come up with a solution for you
Also if you can upload the BobCAD file you are working on that would be a big help
It looks to me like a combination of setting in Mach and BobCAD Post could be the problem. I`ll have a go at your files when I get a bit more time
Regards
Last edited by The Engine Guy; 08-05-2012 at 06:24 AM.
After running your code through Predator backplot the stock was way to big, double the size required, had you run the code at your machine then it would have crashed
Had a quick "play" with your Post, changed it over to Diameter mode and it seems to be working fine now. Here is the line to change in your Post.
249. Output X as a diameter or radius (d/r)? d
Posting code in Radius mode for Mach3 that is running in Diameter mode isn`t going to work
Regards
Hi,
Thanks of this. Based on your earlier post I made the "executive decision" to switch to diameter mode. I set this in both Mach and in BOBCad. I then created a simple part and produced G Code in BOBCad and Mach (using a wizard).
I looked at a few things that were puzzling but eventually spotted a Mach parameter under "ports and pins" - "turn options" - it was "reversed arcs in front post". I had this checked for some reason - unchecking it corrects the arcs in Mach, so I now have BOBCad code that looks like it will run on the machine.
I noted that BOBCad is producing G Code with radius terms rather I and K terms like the wizard for G02 aadn G03. I could change this using line 242 in the post but Macc seems happy with either so I will leave it.
I am doing my Mach testing this evening on my laptop in the office - tomorrow I will go live on the machine (Denford Orac).
I still have something a bit odd in Predator where the stock looks too big - I will chase that down tomorrow and work through your mode suggestions.
Thanks again
Ian
Ian
Sounds like you have most of it sorted now, if you haven`t changed the Post line 249 to diameter then the post is outputting the code at half the geometry, so a line you have drawn at 1 inch will be output at 0.5 so Predator will create a full size stock diameter because that isn`t altered by line 249 and then it runs from the G code at half diameter so it starts halfway down the face of the stock.
If you were to run that code in your machine with 1 inch diameter bar stock then the tool would literally try to go into the material at the 0.5 inch point, fairly disasterous consequences I would say
FYI I also have a Denford Orac Lathe
Do you have the rear tool post for the parting off tool on yours ? ? If so you will need to make some changes to your BobCAD Post and remember to change the tool orientation in BobCAD
Regards
Ok,
Sticking then with the mode issues then I have converted to use diameter mode exclusively. To do this you need 4 things configured;
Mach3 needs to be set to diameter mode - config - ports and pins - turn options - then check diameter mode. Whilst you are here check that reversed arcs in front post is not checked (unless your machine physical configuration demands it).
BOBCad-CAM needs also to be in diameter mode - preferences - settings part - units - highlight lathe diameter mode
Use a post processor that is also set to diameter mode as described by The Engine Guy - post processor line 249. Output X as a diameter or radius (d-r)? set to d
Finally, if you use predator you need the "machine control emulator" (BOBCad probably have a proper name for this file) to be set to diameter mode. In my case I am using FANUC 16TA. You will find the file by following the path - Predator Software\Common Files\RPost 7.0\Lathe then the file you are using .rpl. Towards the end of this file you will see a line lathe_prog_mode=diameter - ensure that this is diameter and not radius. I think that diameter is the default setting here.
With all these things aligned on diameter mode then it looks like everything is working at least on my PC - Next step is to take the G Code to the machine.
Ian
Hi,
Moved onto the machine this morning - first thing is M03 to start the spindle is missing in the code - I think this is in section 2 of the post
n,spsp_code,s
This is outputting N04 G97 S1000
I am scratching a bit here - any ideas?
With a manual spindle on - the code seemed to run ok with no work in the machine - put the job in and re-ran the code.......crash!
Not sure what happened, still licking my wounds.
Ian
Posting Permissions
| | |
