The work holding files are parametrically designed so you can go into the parameters tab to edit the stock size, parallel height and jaw gap.

When you make a new setup you have to select the HAAS UMC 350-EDU model from your machine library. This will bring the physical model of the machine into your simulations so that you can see collisions before they happen. It also tells the post processor the type of machine you are using, which will affect the generated G-code.

When you post process your code there are a few important settings.

• You need to have the 5-axis machine selected, this changes how the G-code is written to make it suitable for the machine. This should autofill if you include the machine in the setup.
• The name/number has to be a number, but which number doesn't matter.
• Don't use "Optionally measure tools at start". It doesn't work and can actually overwrite the length offsets of tools incorrectly.
• Turn on "Optionally cycle tools at start". This puts each tool in the spindle before you run the program, so you can validate you set the tool number correctly. This is important because it allows you to check you got the tool numbers correct, and you can measure the lengths to confirm all tools are probed. After all the tools have been validated you can turn on "block delete" and it won't cycle the tools every time you restart the program.
• Turn on "Safe start all operations". This adds some extra lines of code that make it safer if you start your program part way through. These lines are optional so you have to turn off block delete to make them work. This setting isn't important most of the time.
• Turn on "Use G0". This means rapid move will be output as G0 moves. If you don't turn this setting on, some of the rapid moves will use G1 F5000 instead of G0. It is safer to keep all your rapid moves controlled by rapid override so it doesn't switch from rapid to feed unexpectedly.
• IMPORTANT Change "High feedrate mapping" to "Preserve axial and radial rapid movement". Do not leave this as "Preserve rapid movement".
  • When using tool center point control (TCPC, G234) for simultaneous machining G0 moves including a B and C rotation can cause collisions, and create jerky movement. This setting changes these rotary rapid moves from G0 to G1 F5000 moves, which are safe and smooth.
  • Unfortunately this means some of your rapid moves are controlled by the feedrate override. Just know that your rapids might change from a 5% G0 move to a 100% G1 F5000 move. You might like to reduce your feedrate when stepping in a program but remember to increase it again before cutting.
• All the other default settings should be correct.

The stock is a block of mild steel 65 x 50 x 20 mm. You can find more information such as the % carbon in the data sheet: https://www.edconsteel.com.au/store/sp/bfms.65.20

You should use the small yellow vice to hold the block on both sides. You must always model the vice in Fusion for 5 axis operations to check for collisions between the tools and the vice.

The second operation will clamp onto the dovetails that were milled in the first operation. When constraining the second vice you should ignore the rectangular stock because it has already been machined away. Constrain the second vice directly to the dovetail on the part, which is easier to do with 3 constraints rather than one joint.

You will need to adjust the parameterized stock Y distance to make the vice jaws close perfectly onto the part. If you constrain the part to one of the vice jaws, you can measure the distance between the second jaw and the part, then adjust the stock size to make it fit.

Recommended toolpaths: Adaptive, Flat, 2D contour

Work out what orientation would work best.

Make sure to clear most of the material before finishing.

Recommended toolpaths: Adaptive, Flat, 2D contour

The dovetails have a square corner, so it can be machined with a flat endmill easily.

If you are feeling fancy you can try to use a pattern to duplicate your toolpath from one side to the other. A side note, mirror patterns will reverse climb and conventional.

The dovetail will fit in the vice for op2. Holding onto a dovetail rather than the flat sides of the stock is much stronger, so dovetails can be cut in raw stock for extra work holding strength when machining tall parts.

The dovetails have been designed at a 5 degree angle to the stock, to force you to learn more complex probing for op 2.

Op 1 Recommended toolpaths: Drill (use deep drilling full retract, slightly slower but safer), Adaptive, 2D contour, Probe geometry (in the inspection tab)

Op2 Recommended toolpaths: Manual NC, Probe WCS (look at the probing requirements section of this guide for more information)

For the 12mm hole you must predrill the hole with the 9mm drill and plunge the 8mm endmill through the predrilled hole. This is the best practice to avoid tight ramping or boring, as descending toolpaths will put excessive stress and wear on the flat end of the tool.

We are also going to use this 12mm hole to automatically probe an accurate XY in the second operation so please cut 1mm deeper than it is modelled. Please do not cut though the entire stock, so we can try some different probing routines.

Make sure there are no plunges in simulation, it is easy to mess up the drilling depth.

This hole needs to be milled using wear compensation to create a precise sliding fit for a 12mm dowel/endmill. It should be within a F6 tolerance, which is between 12.016 – 12.027mm. The hole has been modelled in the middle of that range as 12.022mm. This is a tight tolerance, but the machine should be able to do it. This can be done automatically by probing a semi-finished diameter and using wear offsets.

Useful tolerance websites if you have to do this yourself - https://amesweb.info/fits-tolerances/tolerance-calculator.aspx and https://www.mec-engineering-spreadsheets.com/documentation-area/fit-tolerances-and-applications/

I would recommend doing a spring pass to reduce the taper of the hole.

For the wear offset probing to work the semi finish and finish toolpaths have to be identical. Same stepover, same feed, spring pass, etc.

The stepover for semi and final finishing cannot be too small, otherwise the wear compensation can make the stepovers largely different. Imagine a small 0.05mm stepover, if the radial wear offset is 0.015 then the real stepover of the semi finish pass is 0.05 but the final pass stepover is 0.065, a 30% increase. This increased stepover will increase the tool deflection and then the bore is the wrong size.

To get a nice surface finish (and to learn) you are required to do two feed rate compensations in order to maintain the desired chip thickness for the tool. These will be two numbers that you multiply with your original feed rate.

Firstly, adjust for chip thinning due to the small finishing stepover. https://www.machiningdoctor.com/calculators/chip-thinning-calculator/

Secondly compensate for the difference between actual and effective feedrate due to milling a tight curve.

Recommended toolpaths: Adaptive, 2D contour, Trace, Flat

To machine this feature you must use the flat tip of the endmill from 11 different orientations. It is annoying to create a different operation for each orientation and fortunately you don’t have to. You can create the finishing operation for one side then use a circular pattern (under setup) to do the rest. The flats are each 6 degrees apart and the central axis should be under the construction tab. You can also create the axis of rotation by creating two midplanes between any four of the flats, then create an axis at the intersection of the midplanes.

Make sure the tool doesn't gouge into the surrounding stock. To avoid gouging you might have to edit the lead in parameters and design the toolpath to cut close to the center of the tool.

Make the tool lead in from the side of the feature, rather than plunging or ramping down.

Recommended toolpaths: Pocket roughing, Multi Axis finishing, Steep and Shallow, Blend, Flow, Geodesic

Make sure to do a roughing operation with the ball mill before finishing. A roughing operation with the flat endmill leaves a lot of stock so your finishing pass depth of cut will be inconsistent, which creates worse surface finishes.

In this scenario pocket (offset) roughing is better than adaptive. Pocket is designed for small stepdown and large stepovers and will allow slotting. Adaptive is designed for large step downs and small stepovers and won’t allow slotting.

If you would like to you can machine this feature with full simultaneous toolpaths. I would recommend Multi Axis Finishing, Steep and Shallow, Blend, Flow or Geodesic. If using any of the traditional 3D toolpaths try to find ones with the Lead and Lean setting, this is an easy way to control the angle of the tool and prevent cutting on the tip.

It is also sometimes useful to use the avoid surfaces setting or the model setting (with the setup model not included) to prevent the tool from machining the surrounding flat area. These are both in the geometry tab of certain toolpaths.

Recommended toolpaths: Engrave

Please engrave 3+2 into the side of the part.

This is designed to force you to rotate the vice to a 90 degree angle, so that you can see how important tool clearance and accurate holder and vice simulation is.

If we don’t have any coated engraving tools you can do it with an uncoated endmill but make sure to label it for steel, because it will be too dull for aluminium afterwards.