Arccheck? or what's behind Door #2

[Platinum]

I'm trying to tweak my post for the smoothest arc output. I'm getting line/arc combinations in areas that should be arc moves.

 

breakarcs = 1

arcoutput = 0

arctype = 2

do_full_arc = 0 (should be 1?)

helix_arc = 1

arccheck = 1 (should be 2?)

atol = .01

ltol = .002

vtol = .0001

 

What am I missing? Any help would be apprectiated, and many thanks in advance.

[Steve Biehl - Cimquest Inc]

what sort of geometry are you cutting? Is this a contour or surface machining? If you had a wireframe contour with arcs, the above settings would generate arc code. 'do_full_arc' would allow post to generate a single arc command for a full 360 arc.

 

arccheck = 1 has the post check arc length and use ltol. arccheck = 2 has the post check the angle sweep of the arc using atol, = 3 makes it use both.

[Christian Raebild]

What Steve wrote is for using Mp.dll versions prior to version 9.13. The Mp.dll in Mastercam v9.1sp2 is newer than that, so the meaning of arccheck is:

 

1’s

 

1 or 3 – Check the length of the arc to the ltol variable. (This option existed prior to MP Version 9.13. It permits backward compatibility with current post processors.) Note: arccheck : 2 is ignored. (It is the same as arccheck : 0.)

 

10’s

 

10 – Check for motion on the axis parallel to the vector from center point to end and/or start point when the vector is parallel to a quadrant. The move is converted to a linear move if no motion is detected.

 

100’s

 

100 – Check the end point of the arc by using the rounded positions for the arc (center point, start point and sweep) to calculate an end point at machine precision.

 

200 – Perform the test as in (100) but use the generated end point and output the arc.

 

300 – Perform the test as in (100) but the calculated end point is not rounded.

 

1000’s

 

1000 – Check the angles (θ1 and θ2) on the arc formed by the vectors from the rounded start point to rounded center point, rounded start point to rounded end point and rounded end point to rounded center point to the atol variable value. (This option was formerly set with arccheck : 2 in versions of MP prior to v9.13.)

 

Code Example

 

arccheck : 211 # perform options 1, 10 and 200

 

The settings you have should not convert arcs to arcs and lines except for very short arc segments, which might be interpreted as 360 degree arcs by your control if they were not converted. I do not think your problem is on those settings.

 

Note that the setting helix_arc : 1 means helical moves are output as helical arcs in all planes. Unless your post and control supports that, you could get some bad code, causing the tool to go in unintended directions, or causing your machine to stop with an alarm.

[Steve Biehl - Cimquest Inc]

wow !! Christian, is that in the new post pdf's? I'll have to take a look at the new stuff.

[Platinum]

Steve,

I cut 2D contours and 3d contours with wireframe, as well as surface machining.

 

Christian,

I will do some modification to the pst and try that and will have to check on the control for helix.

[Steve Biehl - Cimquest Inc]

platinum,

can you put a example up on the ftp that we can look at?

[steve f]

quote:

---

The settings you have should not convert arcs to arcs and lines except for very short arc segments, which might be interpreted as 360 degree arcs by your control if they were not converted.

---

Christian...this is exactly what has been happening lately with one of my customers. Arc segments with start and end point value differences of .0001" are creating full arcs (and part damage) in the control. What's the fix?

 

thanks for any help,

 

steve

[Platinum]

Thank you

Using "arccheck = 211" certainly seems to reduced my code. Have made a few other "minor" adjustments as well.

How much changing can I do to the LTOL variable before my accuracy goes in the toilet?

[Christian Raebild]

Steve B:

 

Yes, that is straight from the new PDF's

 

Steve F:

 

You need to set arccheck : 1 (or something ending on 1) and an appropriate ltol value, so those short arcs are converted to lines.

 

Platinum:

 

The possible change to ltol depends on what kind of parts you are doing. Basically, an arc with a distance from start to end of less than ltol will be converted to a line, regardless of the radius of the arc. So, with a ltol value of .02, an 180 degree arc with a radius of .01 will be converted to a line, through the center, which causes a deviation of .01 (in addition to the toolpath tolerance).

 

As a side note, on Heidenhain controls (at least older Heidenhain controls), ltol has to be .02 (or greater) when working in metric to prevent unintended 360 degree arcs, if arccheck : 1 is the only check made. I am not certain whether a smaller ltol value can be used if one or more of the other checks are also made, a ltol value of .02 does not result in a unacceptable deviations if the minimum arc radius is set to .05 or higher in toolpath filtering.

[Platinum]

Christian:

Thank you, again. Now I have a better grasp of these tolerances and can do some more modification to my PST.

 

Are the new PDF's with the MR0304 cd? or accessible where?

[gcode]

quote:

---

is that in the new post pdf's

---

Where can I get a copy of this PDF???

[Steve Biehl - Cimquest Inc]

Call your dealer, they can get you the V9.1MR0304 Post CD.

[Christian Raebild]

I think you will have to talk with your dealer about the post PDF's.