MC 2021 issues with flats when cutting curves

[jim1960]

I am making a 2D part that is all curves.  Curves are 1.5" diameter

.75 Z cut, .75 cutter .015 final cut

I am getting small flat spots rather than a smooth curve.

I have cut this type of part on prior versions of MC and not had this issues.

Any thoughts.

[pullo]

one file is worth more than 7600 words 

Gracjan

 

[Guest]

6 hours ago, jim1960 said:

I am making a 2D part that is all curves.  Curves are 1.5" diameter

.75 Z cut, .75 cutter .015 final cut

I am getting small flat spots rather than a smooth curve.

I have cut this type of part on prior versions of MC and not had this issues.

Any thoughts.

What operation are you using?

If you are using pocket operation with a spline,there is a tolerance setting for that usually set to .005, that needs to be lowered .0001 or whatever you need.

[gcode]

are you sure the geometry  you are chaining is an arc?

If it's actually a spline you can get a faceted toolpath.

[Rstewart]

In backplot look to see if you're getting arcs or small straight line segments.  it states this in the information box when you expand it.

 

[Chris In-House Solutions]

If you are chaining an arc and the post is llnearizing the arcs you can try turning on the arc filter tolerance.  On in the control definition the Support arcs in XY, XZ and YZ might be unchcked.  Without a file though its tough to say what the issue is.  

[jim1960]

I am using a contour

Handle.emcam

[JoshC]

hi Jim, that Arc is getting broken up into small lines because the toolpath does not have the arc filter page turned on, to fix this use settings like the ones shown in the image below and it should fix the issue. From my testing the settings i show below work nicely and will produce a nice program

[crazy^millman]

28 minutes ago, jim1960 said:

I am using a contour

Handle.emcam

Thank you for sharing a file. 

[Roger Martin from CNC Software]

 

The arcs in your chain are in View #21 and #22. How did they  get there?
If you create new “Plane from Geometry? and select one of the arcs and display the plane’s gnomon, you will see the issue.
You can "Transform-Translate to Plane" to reorient them to Top.
First, create a point at the center of the left-end arc. We will use that as the Rotation Center Point.
Now do the Translate to Plane…
Select the arcs to be moved.
For the Source Plane select the “Unnamed plane ##” at the bottom of the list.
(If may already be the Source setting as it read it from the selected geometry.)
For the Destination Plane select “Top”.
Now in Center of Rotation select the center point you created for both the Source and Destination,
Click OK (green check) to perform the Translate operation.
 You can verify the arcs with Analyze (F4) to confirm that they are now in View #1 (Top).
Now do Rechain All in the operation to select the relocated geometry.
Regenerate the path and you should get  G2/G3 arc motion in the NC output .

[JoshC]

^Good Find Roger. I didnt even see this when i looked over his file, this explains why i had to manipulate arc filter settings to get mastercam to make an arc.

after reopening his file and turning on his solid, i can see from a top plane his entire part is skewed, looks like his part is sitting on almost a 1 degree angle and is not sitting flat relative to his top plane. so those arcs will be cut as splines since the part is not flat, looks like the big thing he needs to fix here is to rotate the part till the top of the part is parallel to the top plane or create a new plane to work from. 

jim1960 if you go to a Right side view you will see your parts on an angle, fix that and your problem will likely disappear. The fix roger mentioned above sounds like an easy way to fix it.

[jim1960]

Thanks all,

This is a part that was imported and I just did not check well enough

Jim