Note: The B-Axis (Tilt) needs to be at B0 when setting tools with the probe on all UMC and UMC DUO machines. This makes sure that machine rotary compensations (Setting 254) are not inappropriately applied during the tool setting process”
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.
Circular Interpolation at Low Feed Rates:
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.
Circular Interpolation at High Feed Rates:
On a UMC-750, a hole that is circularly 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.
When Drilling From B90 C0 to B90 C180 The Holes Don't 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.
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.
Surface Finish Issues
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.
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. You can also adjust the feeds and speeds to reduce the chatter.
Varying Surface Finish when Cutting 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.
To make this site work properly, we sometimes place small data files called cookies on your device. Most big websites do this too.
What are cookies?
A cookie is a small text file that a website saves on your computer or mobile device when you visit the site. It enables the website to remember your actions and preferences (such as login, language, font size and other display preferences) over a period of time, so you don’t have to keep re-entering them whenever you come back to the site or browse from one page to another.
美元价格不包括关税、报关费用、保险费、增值税及运费。 USD prices DO NOT include customs duty, customs fees, insurance, VAT, or freight.
人民币价格包含关税、报关费用、货运保险和增值税, 但不包括运费。 CNY prices include customs duty, customs fees, insurance, and VAT. DOES NOT include freight.
Haas Delivered Price
This price includes shipping cost, export and import duties, insurance, and any other expenses incurred during shipping to a location in France agreed with you as a buyer. No other mandatory costs can be added to the delivery of a Haas CNC Product.
KEEP UP WITH THE LATEST HAAS TIPS AND TECHNOLOGY...