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-EUD 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 processer 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. The machine was nearly crashed because of this.
• 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 there is no system to the tool number and it is easy for someone else to change a tool unexpectedly. 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 "Use G0". This means all rapid move will be 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.
• All the other default settings should be correct.

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.

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, Flat, 2D contour, Trace

There are a couple different ways to machine this, depending on how much stick out you give your 8mm flat endmill. More stick out is bad because decreases stiffness of the tool by a power of 3 (if you double the stick out the stiffness decreases by 8 times). If you mill the flats with the tip of the endmill you don’t need much stick out, so this is my preference. But it is annoying to create a different operation for each new orientation. Fortunately, you don’t have to. You can create a finishing operation for one side then use a circular pattern (under setup) to do the rest. The flats are each 6 degrees apart. To get the center axis you can create two planes using midplane on some of the flats. Then an axis on the two planes is concentric.

If you don’t want to use the tip of the endmill see if you can find another way to mill this feature, but be careful of collisions.

Recommended toolpaths: Pocket clearing, Scallop, Morphed spiral, 3D Contour, Geodesic

This weird thing can be milled in the normal orientation, but cutting with the tip of the ball mill is not ideal. It causes the ball mill to wear much faster, increases the chance of chipping or breaking a tool and will leave worse a surface finish.

Fortunately, we are using a 5 axis, and so we don’t have to use the tip of the ball mill if we rotate the part. Try using the slope setting that is in most 3D finishing toolpaths to avoid cutting with the tip. Then you can machine the entire surface with two or more orientations.

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.

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 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. Try both and see what toolpath seems more efficient.