How to Use FANUC Manual Guide i engraving Doosan Lynx

FANUC Manual Guide i Engraving on a Doosan Lynx 300M

FANUC Manual Guide i engraving is one of those things that often looks more complicated than it really is.

Now I admit to having a few “issues” with Manual Guide i  but when it comes to engraving I have to admit it’s quire simple.

Not well explained, sorry I’m doing it again. Anyway once you get how it works and what it wants to know it’s easy

If you have a CNC lathe with a C axis and driven tooling, you can do much more than turn diameters and face components. You can mill flats, drill cross holes and engrave text directly onto the component.

Loads and loads of shit. So much fun without taking down your pants.

On the Doosan Lynx 300M, you can engrave on the front face of a component or wrap the engraving around its outside diameter. It can be straight across the front face or rotated around it.

This type of C-axis engraving is ideal for adding:

• Part numbers
• Batch numbers
• Serial numbers
• Company names
• Material specifications
• Inspection references
• Simple identification marks
• And the most common which is rude comments to make your mates laugh

Manual Guide i makes the process quite straightforward. You can create the engraving conversationally rather than calculating and programming every individual movement yourself.

FANUC describes Manual Guide i as a conversational programming system for turning, milling and combined machining applications. You can read more about its capabilities on the official FANUC Manual Guide i website.

What Does the Machine Need?

Before you attempt any CNC lathe engraving, the machine must have the correct tooling.

I’m working on a Doosan Lynx 300M today children and it’s a lovely machine.

Your Machine Must Have

A programmable C axis

Driven or live tooling

Axial driven-tool holders for front-face work

Radial driven-tool holders for work around the diameter

FANUC Manual Guide i

It’s All About the C Axis

The C axis allows the main spindle to be positioned and controlled like a rotary axis.

Instead of simply rotating continuously as it would during a turning operation, the spindle can move to an exact angular position. It can then coordinate that movement with the machine’s other axes.

The driven tool provides the cutting of the letters.

Put those two things together and the lathe begins to behave like a milling machine.

The most confusing thing with engraving is the positioning but once you get this it’s easy.

Fortunately you get to test all this in the graphics. Anyway you might get some weird shit but at least it’s only fresh air.

Engraving on the Front Face

Face engraving on a CNC lathe is normally completed with an axial driven tool.

The tool points towards the front face of the component, parallel to the machine’s Z axis.

The engraving movement is produced by coordinating the machines X axes with the C axis.

Exactly how the operation is displayed will depend on the version of Manual Guide i and how the machine-tool builder has configured the control.

Begin by selecting the appropriate FANUC engraving cycle in Manual Guide i and choosing the front face as the machining surface.

You will then enter the information required by the cycle.

This will normally include:

• The text to be engraved
• Character height
• Engraving depth
• Starting position
• Text direction
• Cutting feed rate

Manual Guide i then creates the necessary tool path.

One important consideration is the amount of room available.

The further the text is positioned from the centre of the component, the more space there is around that radius. Text positioned very close to the centre can become cramped because the available distance reduces rapidly.

Always use the Manual Guide i graphics screen to check the result before running the program.

That little graphics button can save a lot of frustration.

Engraving Around a Diameter

Engraving around a diameter is where having a C axis becomes particularly useful.

For this operation, we normally use a radial driven-tool holder. The engraving cutter points towards the centreline of the component and cuts into its outside diameter.

The Z axis controls the position along the length of the component while the C axis rotates the component.

This allows the text to wrap around the diameter.

You could engrave a part number around a collar, add a company name to a component or mark a round part without removing it from the machine.

The control must convert the linear length of the text into rotary C-axis movement.

The component diameter is important an error in the diameter entered can alter the size and spacing of the completed text.

Choosing an Engraving Tool

For most driven-tool engraving, a small carbide engraving cutter works well.

These are often pointed cutters with an included angle such as:

• 30 degrees
• 60 degrees
• 90 degrees

A cutter with a smaller included angle produces a finer line, but it may also have a more fragile tip.

A 90-degree engraving tool is strong and readily available. However, its cutting width increases quickly as the engraving depth increases.

This is why engraving depth is important. You can even use a spot drill.

You generally do not need to go very deep.

For basic identification work, an engraving depth of approximately 0.05 to 0.15 mm will be sufficient. The correct depth will depend on the material, cutter angle, surface condition and required line width.

Engraving cutters have very small tips and do not enjoy being treated like roughing tools.

Setting the Engraving Tool

The tool must be set accurately but it is no different to any other radial tool so set it in the same way.

For front-face engraving, the tool’s Z length and X position are set.

For engraving around the outside diameter, the radial tool position is particularly important because it controls the actual engraving depth.

A small setting error can make the engraving:

• Too shallow
• Too wide
• Uneven
• Completely invisible
• Much deeper than intended

It is a good idea to prove the Manual Guide i engraving operation on a test component or a scrap piece of material.

Add some to the offset to begin with the tool slightly clear and adjust the offset gradually until the engraving looks correct.

Speeds and Feeds for CNC Lathe Engraving

Engraving speeds and feeds depend on the material and the cutter being used.

A small carbide cutter will often use a relatively high rotational speed. However, remember that the driven-tool spindle on a CNC lathe may not have the same speed range as the spindle on a machining centre. It will probably end up being flat out.

Start conservatively and follow the cutter manufacturer’s recommendations where they are available.

Sometimes the bearings are not too good in driven tools especially when they get older. Might be worth warming it up at around 1000 rpm for a while before taking the speed too high.

These tools should be serviced but no one can ever be arsed to do it. Maybe you will but it’s well worth it.

The cut is normally very light, so the biggest risks are not spindle load or horsepower.

The biggest Risks

• Breaking the cutter tip
• Running the driven tool in the wrong direction, try starting it at slow rpm then take it up, that way you can see it.
• Using the wrong engraving depth
• Selecting the wrong machining surface
• Entering the wrong component diameter
• Starting at the wrong angular position
• Running too close to the chuck, you probably won’t spot this in the graphics.

Check the driven-tool direction before bringing the cutter into contact with the component.

Proving the FANUC Engraving Cycle

Before running the engraving cycle, use the Manual Guide i simulation or graphics display.

Check that:

• The text is spelt correctly
• The text faces the correct direction
• The starting point is correct
• The characters are not mirrored
• The correct machining surface has been selected
• The tool is on the correct side of the component
• The engraving fits inside the available area
• The approach and retract movements are safe
• The tool holder has sufficient clearance, again you won’t spot this in graphics.

Prove the Operation on the Machine:

• Single Block
• Lowest rapid override
• Start with low feed override
• A safe starting position
• You can move datum and machine in fresh air to test.
• Be particularly careful when using a radial driven tool close to the chuck.
• The cutting tool may have plenty of clearance, but the body of the driven-tool holder or turret may not.
• The chuck is unlikely to move out of the way simply because you have made a mistake.
• You may need to reset the C Axis datum so that you miss the jaws of the chuck.
  

  FANUC Manual Guide i

  The main advantage of the engraving feature is that you do not have to calculate and program every letter manually.

  You tell Manual Guide i what you want to engrave, where you want it positioned and how large it should be.

  The control then generates the machining data and allows you to inspect the toolpath.

  That does not remove the need to understand what the machine is doing.

  Conversational programming is there to help the programmer. It is not there to replace checking.

• Graphic can give you a false sense of security. Don’t forget that the grapics does not allow for your tool length. I also knows nothing about the work offset.For more articles about conversational programming, program conversion and using the control, visit the Manual Guide section of the CNC Training Centre website.
  

  All Shapes and Sizes

  First of all on your cutting conditions tab give clearance above your part (C)

  

  Give it your feed rates and then the PLANE SELECTION.

  

  This will give you two choices. It might be helpful to think of C as your Y axis.

  

  This would be the front face (XC)

  

  This would be wrapped around the diameter of your part.

  ZC Result

  This is what ZC would give u

  s

  Position Tab

  Hit the POSITION tab

  

  H-10. means I am 10mm away from the front face of the part.

  V20. is the angle, normally this can be zero but it is where the text is placed around the diameter.

  The base position would be the radius that I am placing the text on. B72.5 would mean I am on a 145mm diameter. Were you to place text on the front face then you would chose XC and this B figure would be zero

  You have a choice of full or half size characters.

  The CHAR SIZE id the height of your lettering

  ANGLE is the angle that the test is at chose the icon

  

  Click the STRING tab and type in exactly what you want to say

  

  Final Thoughts on FANUC Manual Guide i Engraving

  The FANUC Manual Guide i engraving feature is very useful on the Doosan Lynx 300M.

  Because the machine has a C axis and driven tools, it can engrave both:

  • Across the front face of a component
  • Around the outside diameter of a component

  Once the tool has been set correctly and the cycle information entered, Manual Guide i completes most of the difficult programming work.

  The important points are to select the correct machining surface, enter the correct component diameter, keep the engraving depth sensible and check the graphics before pressing Cycle Start.

  As always, prove the program carefully.

  The machine will engrave exactly what you tell it to engrave.

  Unfortunately, this includes spelling mistakes.