Cutting unplanned random circles

[ETC Don]

I'm cutting a leaf that will be a cribbage board.  The leaf contour is made up of many arcs.  One of the arcs continued around as a circle on the CNC, however it did not show up on verify operations.  I read on a couple other forums that it may have to do with truncating values and seeing the starting point of the arc being the same as the end point.  A zero length arc or full circle.  

I'm looking for a way to prevent this.  I don't believe it's very common, but it kinda ruined my project.

[Colin Gilchrist]

Can you post up the file so we can help you identify "where" the error is occuring?

I typically see this happen based on a couple scenarios:

• You have the error you mentioned previously: "rounding or truncation" of arc endpoint values, causing the control to "see" a full-circle (and ruin your part).
• Another possible culprit is "Arc Breaking". I've seen where Mastercam is outputting a "perfectly valid" arc with 90.004 Degrees of Arc Sweep. Because the Control Definition is set to "break at 90 degrees", we get two arcs: one with 90-degrees of sweep, and one with 0.004-Degrees of sweep. This has the same effect of 'causing the control to see a "360-degree arc".
• A final issue that I see come up is related to the above error types: a very small "piece" of arc is created, where a "short line" would technically make much more sense. I see this error come up because > people use the "Filtering Defaults", which are "min arc radius = 0.001" and "max arc radius = 100.". Well, a 100" Radius = a 200" Diameter Arc. Does "an arc that big" make sense for the "size of part" you are cutting? Most often > no, it is much to large for what we're really after > clean arc/line toolpath centerline code.

I'd recommend making the following changes to your Control Definition Settings:

> Machine Tab > Machine Definition Manager > Press [Control Definition] Button > Tolerances Page

• Change "Minimum Distance between Arc Endpoints" = 0.0008"
• Change "Minimum Arc Length" = 0.0012"
• Change "Minimum arc radius" = 0.0004"
• Change "Maximum arc radius" = 321.0" < "set max arc", just remember what you set in case you need to "output" larger arcs to the NC Code File.
• Change "Minimum change in arc plane for helix" = 0.00014" < 1.4 Tenths
• Change "Maximum deviation in calculated arc endpoints from machine grid" = 0.00002" < 20-millionths

> Machine Tab > Machine Definition Manager > Press [Control Definition] Button > Arc (Mill) Page

• Arc breaks > XY Plane (Disable "allow 360 degree arcs checkbox", if it was enabled).
• Arc break options > Break at 180 degrees. (If "allow 360 degree arcs" is "unchecked", Mastercam will automatically break at 180 degrees anyway.)
• Helix Support > Only in XY Plane OR All Planes Supported (either is fine, but this tells the Post "the machine can 'do' a helix".)
• Leave the "Arc error checks" at the default settings. (5 checkboxes > on, off, on, off, on) Always set radio button to "Round end point - break arc on failure".

Having those settings should help reduce errors in the output of the NC Code. All of those "minimum distance" settings will tell the Post to "break an arc into linear segments", if the distances of the arc (in the NCI file) are less than these tolerance values.

The last part of the equation is your "Arc/Line Filter" settings. I would recommend for that finish contour, something like this:

• Total Tolerance 0.0008
• Line/Arc Filtering Settings (ON)
• Smoothing Settings (OFF)
• Set "split" between 'Cut tolerance' (25%) to 'Line/Arc tolerance' (75%). This should give you 0.0002 for Cut Tolerance, and 0.0006 for Filter Tolerance.

Under the Line/Arc Settings:

• Create arcs in XY (G17) on
• One Way Filtering (OFF)
• Minimum arc radius = 0.0008 Inches
• Maximum arc radius = 8.0 Inches

 

[#Rekd™]

Look at your tolerances for Minimum arc radius in the Control definition and the Arc settings.

Colin beat me to it with a more detailed explanation!!!

[ETC Don]

I've attached the text file.

I'm a little nervous going in to the machine manager.  It gives you warnings that everything going forward will be affected.  But I do believe it's the way to go, I just haven't yet.

 

Leaf Cribbage.txt

[Leon82]

1 hour ago, ETC Don said:

I've attached the text file.

I'm a little nervous going in to the machine manager.  It gives you warnings that everything going forward will be affected.  But I do believe it's the way to go, I just haven't yet.

 

Leaf Cribbage.txt

Yes it's telling you you are editing the machine for all of mastercam. It is possible to edit the machine in a local file also.

 

You can use the machine copy plugin to make a backup or copy to mess with.

[Colin Gilchrist]

I would recommend you read the entire thread for "Setting CD Defaults". This is one of the "pinned" threads at the top of the industrial forum, and has a bunch of information about how Control Definition Files work, and how to set the "Default Settings" for a Control Definition.

[PAnderson]

On 1/4/2022 at 10:55 AM, Colin Gilchrist said:

Can you post up the file so we can help you identify "where" the error is occuring?

I typically see this happen based on a couple scenarios:

• You have the error you mentioned previously: "rounding or truncation" of arc endpoint values, causing the control to "see" a full-circle (and ruin your part).
• Another possible culprit is "Arc Breaking". I've seen where Mastercam is outputting a "perfectly valid" arc with 90.004 Degrees of Arc Sweep. Because the Control Definition is set to "break at 90 degrees", we get two arcs: one with 90-degrees of sweep, and one with 0.004-Degrees of sweep. This has the same effect of 'causing the control to see a "360-degree arc".
• A final issue that I see come up is related to the above error types: a very small "piece" of arc is created, where a "short line" would technically make much more sense. I see this error come up because > people use the "Filtering Defaults", which are "min arc radius = 0.001" and "max arc radius = 100.". Well, a 100" Radius = a 200" Diameter Arc. Does "an arc that big" make sense for the "size of part" you are cutting? Most often > no, it is much to large for what we're really after > clean arc/line toolpath centerline code.

I'd recommend making the following changes to your Control Definition Settings:

> Machine Tab > Machine Definition Manager > Press [Control Definition] Button > Tolerances Page

• Change "Minimum Distance between Arc Endpoints" = 0.0008"
• Change "Minimum Arc Length" = 0.0012"
• Change "Minimum arc radius" = 0.0004"
• Change "Maximum arc radius" = 321.0" < "set max arc", just remember what you set in case you need to "output" larger arcs to the NC Code File.
• Change "Minimum change in arc plane for helix" = 0.00014" < 1.4 Tenths
• Change "Maximum deviation in calculated arc endpoints from machine grid" = 0.00002" < 20-millionths

> Machine Tab > Machine Definition Manager > Press [Control Definition] Button > Arc (Mill) Page

• Arc breaks > XY Plane (Disable "allow 360 degree arcs checkbox", if it was enabled).
• Arc break options > Break at 180 degrees. (If "allow 360 degree arcs" is "unchecked", Mastercam will automatically break at 180 degrees anyway.)
• Helix Support > Only in XY Plane OR All Planes Supported (either is fine, but this tells the Post "the machine can 'do' a helix".)
• Leave the "Arc error checks" at the default settings. (5 checkboxes > on, off, on, off, on) Always set radio button to "Round end point - break arc on failure".

Having those settings should help reduce errors in the output of the NC Code. All of those "minimum distance" settings will tell the Post to "break an arc into linear segments", if the distances of the arc (in the NCI file) are less than these tolerance values.

The last part of the equation is your "Arc/Line Filter" settings. I would recommend for that finish contour, something like this:

• Total Tolerance 0.0008
• Line/Arc Filtering Settings (ON)
• Smoothing Settings (OFF)
• Set "split" between 'Cut tolerance' (25%) to 'Line/Arc tolerance' (75%). This should give you 0.0002 for Cut Tolerance, and 0.0006 for Filter Tolerance.

Under the Line/Arc Settings:

• Create arcs in XY (G17) on
• One Way Filtering (OFF)
• Minimum arc radius = 0.0008 Inches
• Maximum arc radius = 8.0 Inches

 

Colin is correct. I have posted in this very issue and received help from Colin. Thanks Colin, very good information.

 

Paul

[Leon82]

We have ours at min arc rad at .002 and arc length at .002.

 

One guy just had this happen but Camplete didn't report a collision. Bit it shows a weird loop in the path plot display.

 

I'll have to check the arc page.

[#Rekd™]

41 minutes ago, Leon82 said:

We have ours at min arc rad at .002 and arc length at .002.

 

One guy just had this happen but Camplete didn't report a collision. Bit it shows a weird loop in the path plot display.

 

I'll have to check the arc page.

Had this happen and Vericut didn't catch it....they sent a tech in here an investigated...a software update was sent out soon after. It now gives a warning. 

On some files I have to bump the min arc Rad to 0.01" to get rid of the warning.

[PAnderson]

19 hours ago, Leon82 said:

We have ours at min arc rad at .002 and arc length at .002.

 

One guy just had this happen but Camplete didn't report a collision. Bit it shows a weird loop in the path plot display.

 

I'll have to check the arc page.

Camplete will only report a collision if the part file is loaded in with the simulation file and the cutter invades the part. Otherwise, it's just another cut. Easy to have happen if the error shows up early in the stock cutting while not touching the part.

[Leon82]

1 hour ago, PAnderson said:

Camplete will only report a collision if the part file is loaded in with the simulation file and the cutter invades the part. Otherwise, it's just another cut. Easy to have happen if the error shows up early in the stock cutting while not touching the part.

We use the plugin and it took out one of the legs.

 

It was fine the first time then he expanded the optirough boundary on the next part