1. 3d Machining- hsm

2. Machining Strategy
Before starting our machining definition we need to decide on how it is to be machined. Several things affect how this is to be approached:
Finished part or vacuum form
Material (Aluminium, Steel or Pro-Lab)
Shape and complexity of the part.
Part A
Part B
Impossible to profile past this point due to undercut
In the example above, the part is to be machined as a finished part. It is impossible to machine under the part and so it needs to be split into 2 operations. As this part is decorative, the decision was made to machine 2 separate halves and glue them together along the split line.
The part will need to roughed out to an approximate shape and then 3D machined to finish it.
If the part was to be machined as a solid, thought would have to be given as to how to orient the part, hold it and accurately datum up the part when it is flipped to machine the second side (part B).

3. Finished part or Vacuum form tool?
In general, a finished part would be aligned with the flat surface to the bottom of the stock and then machined to thickness.
A Vacuum Form tool would be aligned to the top surface and the remaining material left at the bottom of the part.
Part Holding Strategies
Part held in vice on excess & machined
Part screwed to base board (for Vac form)
Part screwed to base (Finished part)
Part on vacuum table (for Vac form)
The part is to be 3D machined, as the material is oversize and it fits in a vice (<150mm wide) the excess is clamped and the part 3D adaptive milled & finished using a 3D parallel machining strategy. As this is a vacuum form tool, the excess does not matter due to the part requiring trimming after forming.
If this was a finished part, the material would need to be removed from the bottom manually.
The part is to be 3D machined, and is a finished part. As before the part is screwed to a base board but is aligned to the bottom face to allow the part to be machined to thickness. As the cutter will need to pass deeper than the depth of the part and into the base board. The base board therefore needs to be thicker than the radius of the tool +5mm (i.e. a 20 ballnose would need a minimum base board thickness of 15mm (R10+5mm)
To recap:
VMC Vice or on table attached to base board
ROUTER Attached to base board or on Vacuum table
VMC Metals or plastics/Pro Lab
ROUTER Wood or Pro Lab (NOT MDF)
VMC Max size 500x400x300
ROUTER Max size 1200x1000x120 (Vac table 500x400)
The part is to be 3D machined, If there is not sufficient material to hold in a vice (or it is too large) then the part can be attached to a base board which can then be clamped to the machine table. Usually we use 4 #8 or larger wood screws and screw through from the underneath of the base board into the model material. It is crucial that these screws are situated where the cutter will not hit them and that they are recessed into the base board. Failure to do so will scrap the cutter and most likely your part.
Parts held on the vacuum table do not require a base board but must not be machined past the bottom of the part.

4. Starting our part program
The templates for all of the setups can be found at: Teachdoc-LDS>CNC machining Templates>Solidworks
Tools are in here
Router with base board (use for XYZ Too)
Copy the correct template to the desktop, work from there and copy back to your drive space when you are done. Do try to work direct from the network.
Router with Vacuum Table
XYZ with Vice
Open this in Solidworks, this is our manufacturing file.

5. Rebuild Button
Change the material stock to the size of your material. To do this double click on it and then select the dimension and alter. Once done hit the rebuild traffic light to change the block. The base board will also change to the required size.
Open up the drawing file located in the folder, this will give all the details of the required base board, use this to correctly order your board.

6. Next we need to add the part to be machined into the assembly
Next we need to add the part to be machined into the assembly. If you have been working in any other CAD system (Creo, Rhino etc) Output the part by saving as a .STP file. Open this in Solidworks and if asked, run diagnostics and attempt to heal any errors. Save this part as a solidworks file.
Use the mates to align the part (same as in creo). In the example below I align the top 1mm below the top surface to allow it to be milled and then set the 2 sides in by a distance to allow material all round to machine. If this was a finished part I would have aligned the bottom face with the bottom of the block.
From the assembly tab, select Insert Components. If it is already open you’ll see it in the list
The part should be fully constrained before you proceed.
You need to constrain the 6 limits of freedom :
3 Axial, 3 Rotational.

7. Each setup is considered a job
Each setup is considered a job. A job is the full machining sequences up till you would take the part off and reposition or redatum it. To all intents and purposes you should have one job in your file.
Depending on which template you’ve selected, you may have to start a job by selecting “Job”, otherwise it’s already in your history tree.
If you don’t have this in the list…
… click this to add it…
… then right click on the job and select “Edit”.
Select the technology you are using, for a 3 axis machine it’s milling. For our 5 axis router or lathe it would be Turning/Mill-Turn
Select the part to be machined i.e. your part model
As we already have the material modelled as a solid, change the option to “From Solid”
Select the material stock. This is easiest done from the feature tree.
There is no need to fill in this, but it is either the base board, vacuum table or the vice assembly.
Of vital importance is the datum. By default we use a coordinate system which should be modelled at the bottom left of the part and on top of the stock. Make sure Z is upward and X runs along the front face.

8. Tooling
Depending which template you select, you may have to define your tools. There are some tooling packages already which can be imported.
1) Select Tool Library
2) Right click on the part in the open documents tree
3) Select “Import Tools from Library”
4) Navigate to the tooling packages folder and select the correct package

9. Defining your own tools
You may have to define tooling specific to you requirement. It is important that the tooling and holders match what you are planning to allow the simulation to show if there are any clearance issues. Whilst this is not necessary for 2D milling it is vital for 3D milling.
From the tool library screen, select “New Mill Tool”
Define the tool by running left to right and filling in the information on the tabs. Select the tool holder from the Holders sub menu. For example the standard tool holders we use on the XYZ are CAT 40 ER 32. For the router select a CAT40 ER 16. You may need to alter the dimensions or fully define the holder, which is under the Holder Geometry tab but these should be close enough.
Fill out the feeds and speeds, these can be overwritten in your sequence definitions later if required.

10. Roughing the part
Making the 3D part is usually quite simple. Usually it involves roughing out the shape using a slot drill, you may have to re rough it before finishing to remove any areas that a larger slot drill cannot get to. For 3D machining use the 3D adaptive clearing sequence.
These are considered 3D roughing cycles
These are considered 3D finishing cycles
You may also use any of the 2D cycles, for instance use Face milling to remove the top excess material.
Things to consider:
If you are machining deeper than the tool will allow, The tool needs to be sufficiently large enough to clear the tool holder nut. Generally we use a 32mm cutter on the router to allow for this.
The tool used for roughing should be no larger in radius than the diameter of the finishing tool if it leaves internal corners. Ideally use roughly the same diameters for roughing and finishing. You may need to re rough the part with an additional cutter to allow for the radius it leaves
If you have sharp transition between a face and a 3D slope the roughing tool will rough out as close as it can, the finishing ballnose will leave an unmachined area. Model the resultant fillet in your model to avoid unexpected errors.
Roughing tool has roughed out up to the corner, Finishing ballnose will not finish this area. Model the cutter radius in your model to prevent the roughing tool from machining this if it is a problem.
Roughing tool Diameter
The roughing tool is too large (or the finishing tool is too small), this area is not machined and can break the tool, The radius of the rougher should to be smaller than the diameter of the finisher.
Finishing tool Diameter
Top View
Front View

11. Adaptive Clearing
Adaptive clearing works be removing layers of material up to the silhouette and then back machining up from there in defined heights to refine the roughed out shape. It is a very efficient roughing cycle and should be enough to rough out your part.
Select the roughing tool from the library. You can also define or import tooling direct from the sequence.
As we are machining the entire block (and it knows whew the model and stock are from the job setup) we can pretty much ignore this tab. If more intricate machining is required then more definition may be required.
The most important tab is the passes tab. This is where we fine tune how the sequence operates.
Initial roughing step depth
As with all sequence definitions, work left to right across the tabs and fill in the required fields.
I suggest filling in the minimum required, then simulating and the altering as required
Back cut depth (to refine the shape)
Router: (Jelutong or Pro Lab)
Roughing 32mm Slot
Speed: 10,000 RPM
Feed Rate 1500mm
Rough depth 10mm
Back cut 3mm
Stock (Side) 3mm
Stock (Base) 3mm
XYZ: (Pro Lab)
Roughing 10mm L/S Slot
Speed: 3500 RPM
Feed Rate 4500mm
Rough depth 30mm
Back cut 5mm
Stock (Side) 3mm
Stock (Base) 3mm
Material to leave for finishing
XYZ: (Aluminium)
Roughing 10mm Slot
Speed: 5100 RPM
Feed Rate 1000mm
Rough depth 5mm
Back cut 1mm
Stock (Side) 0.25mm
Stock (Base) 0.25mm
Every other setting you can ignore.

12. Finishing the part
The shape is now roughed. To finish it we need to use a 3D machining strategy. Dependent on the form this will vary but pretty much any shape can be achieved by using the parallel strategy. This works in a similar way to how Creo used to 3D machine.
Select the Parallel finishing sequence from the 3D milling drop down box.
Some things to note:
Straight sides should not be machined using a surface milling cycle. Use a 2D sequence (probably contour milling).
Ball nose cutters will plunge past the bottom of the part, you need to:
a) allow for this in your fixturing (so don’t use 10mm thick base board for a 20 dia cutter, it will mill it all away!
b) allow for additional length when choosing a cutter (so if a 20 dia cutter will go 100 deep it will actually plunge to 110 so 90 deep max is achievable.
c) NEVER parallel mill using one axis (0deg or 90 deg. ALWAYS mill at 45 degrees)
Select the finishing tool. For 3D profiling it is usual to use a ball nose cutter. Don’t forget the selection criteria from the previous pages.
If we’re machining over the entirety, once again this can probably be skipped.
As we wish to machine the straight sides using a contour, the outer boundary has been selected.
To ensure the cutter fully machines the surfaces we tell it to machine so the centre line of the cutter hits the boundary.
In addition we have told it to go past by a value
Under the passes tab, we can define how rough we want the surface, to do this change the step over value to achieve the desired cusp height. For a finished surface requiring less sanding you should aim for a cusp height of 0.05mm. The trade off here is the amount of time it will take to machine. Check this out in your simulation.
All parallel strategies should be done at 45 degrees, this splits the load across multiple axes, gives the machine more time to accurately position and so gives a more accurate profile.
As this is a finished surface, make sure stock to leave is unchecked.

13. Creating code for the CNC machines
Post Processing
Creating code for the CNC machines
We have so far created a list of commands which describe how to machine the part, this is not something we can transfer to the machine.
To do this we post process the commands and create code for whatever machine we are running the part on.
Highlight the job (or select all the processes requiring outputting) and select Post Process from the command bar.
In the project folder the post for the XYZ is in the post folder, If we wished to output to the Denford, we could navigate to that folder containing it.
Give our program a name (I’d suggest group number and description)
Hit Post to output

14. Done? Not quite! Creating a Setup Sheet
So we have our code ready to put into the machine, but how do we know where the datum is, what tooling to use, even which way in the vice the part is located?
We need some set up info.
From Solidworks, highlight the job and select Setup Sheet from the command line.
This will create a HTML file with all of the relevant information. This can be printed for referral when setting the machine.