UMC - Common Applications Problems

UMC - Accuracy Error - When Drilling from B90 C0 to B90 C180 the Holes do not Line Up

On a UMC-750, when using a drill from two sides of a part you can get up to 0.002 inch (0.051 mm) error per side. This can add up to a total of 0.004 inch (0.102 mm) mismatch between the two drilled holes.

Use a probe to get separate offsets for the B90 C0 and B90 C180 side.  This can reduce this mismatch error.

UMC - Accuracy Error - When rotating from B0 C0 to B90 and Cutting with the Bottom of the End Mill

On a UMC-750, it is normal to see up to 0.002 inch (0.051 mm) of mismatch between the side cut at B0 and the end cut at B90.

This error can be reduced by probing the location at B90.

UMC - Accuracy Error - When drilling Holes at B0 C0 and Moving the X, Y to Position the Drill

You can expect less than a 0.001 inch and (0.025 mm) error in positioning in the X and Y axis when drilling holes at B0 and C0.

UMC - Accuracy Error - Circular Interpolation at Low Feed Rate

When circular interpolating a hole at low feed rates, you can expect a circularity error of up to 0.001 inch (0.025 mm) when the program has a finish pass.

If the hole has a circularity tolerance less than 0.001 inch (0.025 mm). You will need to use a reamer or boring head to reduce this error.

UMC - Accuracy Error - Circular Interpolation at High Feed Rate

On a UMC-750, a hole that is circular interpolated at high feeds can be undersized up to 0.006 inch (0.152 mm) depending on the feed rate and size of the hole.

This can be caused by:
  • Incorrect Notch Filters parameter values. To fix this, make sure the Notch Filters parameters have the correct values (parameters 884 through 889).  These values are set correctly in the current version on NGC software.
  • The program feed rate is too high for the circle being cut. To fix this, slow down the feed rate.

UMC - Dwell Marks - During 5-Axis Machining

On a UMC-750, the face of the platter can bow or flex up to 0.001 inch (0.025 mm) when the C axis brake is engaged or released.

When doing simultaneous 5 axes machining, it is recommended to release the B and C axes brake ( M11, M13 ) before engaging the tool in the part.

Then engage the B and C axes brake ( M10, M12 ) when the simultaneous 5 axes machining has finished.

UMC - Chatter Marks

On a UMC-750, the tool is more likely to chatter when the Y and Z axes are fully extended.
When this happens, move the part toward the center of the Y axis and up in the Z axis.  Also adjust the feeds and speeds to reduce the chatter.

UMC - Surface Finish - During a Cut Along the X and Y-Axis

On a UMC-750, you will typically get a slightly different surface finish when cutting along the X and Y axis.
This is due to the fact the Y axis is more rigid than the X axis.


These differences in surface finish can be minimized by adjusting the feeds and speeds or using a different cutter with less cutting pressure.
Associated Troubleshooting Content: 

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.