Re: [Emc-users] Getting arcs as G2/G3 moves in g-code?

[Dale <da...@1s...>]

I'm not sure where to jump in here but, EMC's handling og cutter comp 
and inside corners as of my last look doe's need fixing. While I haven't 
used them for many years now, that means it's not a new idea or concept 
. Fanuc was doing it long ago. I could program the exact part profile 
with proper leadin's and leadout's then enter the tool diameter and the 
control would compensate for the tool diameter. Using look ahead which 
EMC already does an it would handle the indide corners of rectangular 
pockets with no problem. No corner radius was required. The only 
exception to that was in contoures where the line segments were too 
short and the amount of tool offset would cause a condition where a line 
segment would be missed completely by the tool. There is a simple cure 
for that, simply skip that line segment and look for the next line 
segment where a tangent can be found. cutting with the cutter on the 
opposite side of the same countour would not cause the problem of no 
tangency (tool will not fit) problems at all. The other thing I think 
EMC needs is Work Coordinate Offset Rotation, It is very nice to use a 
probe to find the g54 - g5n.n origin by touching 3 points for x - y zero 
and one more point to find top of part for z zero. The angle the part is 
clamped to the table can automatically adjust all x - y values of the 
program. The auto skew adjustment works in part program run modes and 
MDI while Manual moves can optionally work with the skew of the part or 
remain true to the machine coordinate system. There needs to be a way to 
tell EMC when probing whether you are probing three points inside a 
circle or two points along one side of a part feature and one point on 
another side that is 90 degrees to the first so EMC can either calculate 
  the center of the circle or the corner. In the event of the circle the 
for part skew ther would be two more points to probe of a planar 
reference surface. Like I said earlier Fanuc (Secos) was doing this at 
least 10 years ago.

   It did not take long to get spoiled by a control that worked in this 
manner. Think about it. No indicating a part to be squared to the 
machine axis or to find center of a bore or the corner for part program 
zero. What a time saver! BTW they also had a tool setter for touching 
off and setting tool length offsets.

Dale


Andre' Blanchard wrote:
> At 01:02 PM 7/30/2007, you wrote:
> 
>>On Mon, 2007-07-30 at 12:04 -0500, Jon Elson wrote:
>>
>>>Dave Engvall wrote:
>>
>><snip>
>>
>>>>My local approach (read fix) is to declare a zero diameter tool and
>>>>then modify my tool table.
>>>>
>>>>Maybe one of the developers can explain how easy or difficult this
>>>>would be to fix/implement.
>>>
>>>I don't think it needs "fixing".  It requires you to select
>>>lead-in and lead-out points that do not contain inside corners,
>>>and is strict about this.  I have gotten it to work fine.
>>>Section 20.4 of this document
>>>http://www.linuxcnc.org/docs/EMC2_User_Manual.pdf
>>>shows how it works.
>>
>>
>>        Jon, I agree with you.  The way G41/G42 and the material-path
>>tangential travel requirements are implemented in emc2 make sense to me
>>(after about 10 hours of digging in, which I consider to be a pretty
>>short curve, thanks to good docs).  I don't think it needs fixing
>>either, unless there's a bug in the G41/G42 stuff, but I haven't
>>detected any.
> 
> 
> It needs fixing only from the point of view that it works in a manner 
> unlike many machine controls in the industry.  With most controls there are 
> a lot more options for different kinds of compensation.
> 
> This code will run on any control I have used as long as the value in the 
> radius comp is less then 2" and if the interference checking is turned off 
> it would work even with larger end mills, it would just cut backwards and 
> leave and oversize hole.
> But EMC will not get past the G41 line making using comp on internal shapes 
> a more complicated dance.
> 
> G00 G54 X0.0000 Y0.0000 Z1.1000
> G01 Z-1.0000 F20.0
> G01 X-1.0000 Y0.0000 G41 D1
> G03 X1.0000 Y0.0000 I1.0000 J0.0000
> G03 X-1.0000 Y0.0000 I-1.0000 J0.0000
> G01 X0.0000 Y0.0000 G40
> 
> 
> 
> 
>>        I do like the earlier suggestion about providing the option of
>>enabling/disabling the tangential contact requirements, if that is not
>>too difficult.  Not because there's anything wrong with how it's
>>implemented, but just because there may well be situations that I know
>>tangential contact isn't going to be maintained, and I'm fine with that.
>>If it could be set in the .ini file, that would be very helpful.
>>Setting it in g-code would be even better, but I realize that would
>>start to introduce non-standard things into the interpreter and is
>>probably not a good idea.
> 
> 
> In industry that is a very standard option.
> __________
> Andre' B.  Clear Lake, Wi.
> 
> 
> 
> -------------------------------------------------------------------------
> This SF.net email is sponsored by: Splunk Inc.
> Still grepping through log files to find problems?  Stop.
> Now Search log events and configuration files using AJAX and a browser.
> Download your FREE copy of Splunk now >>  http://get.splunk.com/
> _______________________________________________
> Emc-users mailing list
> Emc...@li...
> https://lists.sourceforge.net/lists/listinfo/emc-users
>