12. Relief Machining

ArtCAM 12. Relief Machining

12. Relief Machining

Relief Machining.

To physically perform a machining operation on an ArtCAM model a suitable toolpath file must be created and exported in the correct language to the machine tool controller. This file contains a sequence of instructions for the CNC machine to control Tool movement, Spindle Speeds and Feed Rates relative to a defined machining origin.

All of the machining commands are located in the Toolpaths page, accessed by clicking the Toolpaths tab.

The Toolpaths page is segregated into four main categories including Toolpath Operations, 2DToolpaths, 3D Toolpaths, and Toolpath Simulation.

When a toolpath is created it will be displayed in the graphics area and the filename registered in the area to the top of the Toolpaths page. These filenames are selectable for such actions as Toolpath Simulation, or to reopen the original machining form for editing purposes.

A comprehensive Tool database is accessed from within the individual toolpath strategy forms. The user can add to or modify the stored tool definitions as required.

If the NC machine has an automatic tool changer toolpath strategies with different tool definitions can be output to one file. Otherwise it will be necessary to create separate files containing toolpaths with a similar tool definition.

Note: It is often required to modify the origin of the model to a position more appropriate as a machining origin. This is achieved by inputting suitable X Y Z values in the;

Assistant - Model - Set Model Position form.

3D Machining Example

The following example produces a set of suitable 3D Toolpath strategies to machine a stored ArtCAM Relief (teddy bear). The two main 3D Machining strategies Z Level Roughing and Machine Relief can be applied either to the Whole Model or within Selected Vector areas.

The general idea is to first use a relatively large roughing tool (End Mill) with the Z Level Roughing strategy to remove as much material as quickly as possible to reveal a stepped, oversize component form. A suitable finishing tool (Ball Nosed) will then be applied with the Machine Relief strategy to track over the component contours as an initial semi-finishing operation. This tool will be too large to pick out any fine detail or internal corners but will quickly remove most of the remaining stock down to 0.5mm from the component form.

A further Machine Relief strategy using a smaller Ball Nosed tool will then be applied to machine to finish size and pick out the fine detail.

Use the File menu to Close any open ArtCAM models.
Select Open Existing Model.
Select the model Sculpt_Teddy.art from Examples\Ted_bear.

The following Relief appears in the 3D View window:

Before any toolpaths can be created the Material Setup must be defined. The user decides on and inputs a suitable Z position for the relief within the material block.

The X Y dimensions of the material block are the same as those defined in SetModel Size.

Press F3.
Select the Toolpaths tab.
Click the Material Setup button on the Toolpaths page.

The Material Setup dialog box appears:

This dialog box allows the user to input the Z position of the relief within the material block.

The X Y dimensions of the Material Setup are the same as the values defined in Set Model Size.

The Material Z Zero (machining origin) can be s set to the Base or the Top of thematerial block.

Note: If a different XY origin position to that used for the relief creation is required then this is input in the Set Model Position form (see previous page).

As the Relief height is 5.115mm, input a MaterialThickness of 6mm.
Set a Top Offset of 0.25mm (or drag the model to the top using the slider).
Ensure that the Material Z Zero is set to the top of the block.
Click OK.

A Pink outline, representing the material block, appears around the relief in the 3D View.

The machining origin is displayed by switching on the Origin icon located at the top of the 3D window.

Z Level Roughing

Z Level Roughing will remove the excess material from around the relief up to the specified Material Allowance and Tolerance values. For efficiency a relatively large tool is generally used for this operation. Z Level Roughing splits the Material into Z Slices and performs the selected area clearance strategy (Raster or Offset) on each one.

Select the Z Level Roughing button on the 3D Toolpaths section.

The Z Level Roughing page appears.

As with all the Assistant pages the Show Help button can be clicked to show or remove the help from the page.

Select Complete Relief.
Click the Select…button on Roughing Tool to access the standard Tool Database.

The standard Tool Database contains a large selection of tools and associated parameters for a variety of materials. The selection can be modified, deleted, or added to by the user as required.

The Tool Database can also be accessed independently by selecting the icon in the Toolpath Operations.

Select the End Mill6mm from Aluminium – Roughing and 2D Finishing.

When a tool is selected (highlighted) in the left hand window, information relating to it is displayed on the right-hand side of the form.

Individual tools are altered using the buttons on the right hand side of this form. Once the tool is altered in the database, it is altered permanently.

Click the Select button to select the tool.

The tool is automatically loaded into the page.

Select the down arrow on the tool to see the tool values.

An end mill tool is generally selected for roughing as it has a flat bottom and it can be stepped over by at least 70% of the tool diameter, reducing the machining time.

The stepover value is the distance the tool moves over between passes. The smaller the stepover, the more passes it will take and it will take longer to machine. For a fine finish will a ball nose tool, the stepover value is around 1% of the tool diameter.

Set the Stepover to 4mm.
Set the Stepdown to 2mm (This will be used for calculating the Z Slices).

Leave Add Ramping Moves unset.

Ramping Moves are frequently used where hard materials are being machined or in cases where a specific tool is likely to break if it is allowed to plunge directly into the material before machining the relief. If Add Ramping Moves is switched on it provides access to a selection of ramping options.

The material is already defined, but you have the option to change it within the machining command, if necessary.

The material and the relief information are loaded into the page.

It is possible to specify initial and final heights for the Z Slices between which the Step Down value applies. Any values entered are absolute relative to Z Zero, which in this case is the Top of the Block.

Leave the Start/Surface Z at 0. (This is the initial height from where the first Step Down value will be subtracted).
Set the Material Allowance to 1.0. (This is the amount of material to be left on the ArtCAMrelief).

The Material Allowance is the specified thickness of material that is left on over the actual relief when the toolpath is created.

The Last Slice Z defaults to the height of the Material Allowance above relief base level. This value can be modified upwards to leave more material on the base level if required.
Click the Apply button.

When you click the Apply button it works out the number of Z slices, based on the tool stepdown and the thickness of each slice. For example, if you wanted to have more z slices, you would decrease the stepdown distance.

Set Safe Z at 5 and the Home Position as X0 Y 0 Z 5.

In this case the origin was set to the top of the material, rather than the base as the diagram shows. The SafeZ of 5 is therefore measured upwards from the top of the material. The Safe Z is the height in Z above the material that the tool can safely move at high speed around to move to the next point of the machining.

The tool home position is the position where is starts from at the beginning of the machining and where it returns to at the end of the machining. This position needs to be at SafeZ or higher

Leave Tolerance at 0.01

Tolerance determines how accurately a cutter path follows the true shape of the relief, the actual value being the maximum permissible deviation from the relief form.

The next stage is to select a suitable Strategy from either Raster or Offset.

Raster Machining

With the Raster strategy, the tool moves across the Z Slices in parallel, straight line moves separated by the Step Over distance. The toolpath is automatically limited away from the relief by the tool radius plus the Material Allowance, as shown.

The Raster process on it’s own tends to leave steps around the relief. If required these can be removed by applying a ProfilePass either before (First) or after (Last) the Raster moves.

Offset Machining

With the Offset strategy, the tool moves are offset inwards from the shape of the Complete Relief or limiting vector, and outwards from the shape of the relief contour. Individual tracks are separated by the Step Over distance.

In this example the Z Slices will be machined using a Raster strategy without the addition of a Profile Pass.

The default Angle - 0 (along X)for the Raster strategy can be changed if required.

Leave the Strategy options as Raster, Angle 0 with Profile Pass set to None and enter roughing for the toolpath name.
Click the CalculateNow button and then Close.

The Toolpath can be calculated Now or Later. When the option Later is chosen it will save the uncalculated toolpath until the Batch Calculate option is selected from the toolpaths menu.

For example several unprocessed toolpaths could be Batched ready for calculation at a later time such as during the users lunch break or overnight.

ArtCAM generates the toolpath as red lines in the 3D View. The dark blue lines are rapid moves in SafeZ and the light blue lines are plunge moves.

The resultant toolpath is displayed along with the relief and Material Setup in the 3D View. The Items to Display button at the top of the 3D View controls which entities are displayed on the screen.

Click the Items to Display button on the 3D View Toolbar.

Different objects are toggled for selection by clicking on them followed by pressing Apply to display the selected items.

Select the roughing toolpath only and click Apply.

The toolpath is now the only displayed item.

Select all and click Apply.

Semi Finishing Toolpath

Next the Machine Relief option will be applied to create a semi-finishing toolpath using a Raster in X strategy with a material Allowance of 0.5mm.

Select Machine Relief on the 3D Toolpaths section.

This machining page covers a variety of semi finish and finish machining options.

Area to machine – this either applies to the Whole Model or the area within the Selected Vector.

Strategy - there are four basic strategy options:-

Raster in X – Creates the strategy along one direction.

Raster in X and Y – Repeats the strategy at 90 degrees.

Spiral - Creates a spiral strategy limited by the model.

Spiral in a box - Creates a spiral strategy trimmed to the model.

Raster Angle – A different Angle can be entered for the orientation of the Raster strategies (default 0 = along X).

Do Multiple Passes - if a hard material is to be machined, instead of applying one heavy cut to full depth, it can be slowly taken off in stages by repeating the strategy downwards from a defined height by applying DoMultiple ZPasses.

Select WholeModel and a Raster in X strategy with a Raster Angle of 0, allowance of 0.5 and tolerance of 0.01.
Set the Machine Safe Z as 5 and the tool Home Position as X0 Y0 Z5.
Click the Select button to select the tool.
Select the Ball Nose3mm from Aluminium – 3D Finishing.

A ball nosed tool is used for semi-finishing to get close down to the model and remove the material left on from the Z level roughing. This is used when you are finishing with a fine or small tool that cannot cut large chunks of material without breaking.

Edit the tool stepover to 0.2 and leave DoMultiple passes unticked.
Enter the toolpath nameSemi Finish.
Click Calculate Now and then Close.

The toolpath has been calculated and is quite fine.

Note: if you need to increase the flat area to make room for the tool to finish off cutting the model, use the Add border command from the Model pull down menu.

Finishing Toolpath

For finishing, a small tool is usually used with a small stepover and an allowance of 0, meaning that it will not leave any excess material on the model. A Machine Relief strategy using a Spiral in Box with zero Allowance will now be applied.

Select the Machine Relief button on the Toolpaths page.
Select Whole model with a Spiral in Box strategy with an Allowance of 0.0, and a Tolerance of 0.01.
Select the Ball Nose1.5mm from Aluminium – 3D Finishing.
Set a Stepover of 0.1.
Name the Toolpath Finish.
Click Calculate Now and then Close.

The generated toolpath is as shown. This strategy, which is very good for circular shapes, does produce lots of tool lifts which can slow down the machining process.

Machining Local Areas

If required it is possible to restrict the machining to an area bounded by a vector.

In this example the area around the eyes and nose would benefit from a further Finishing strategy using an even smaller tool. A closed Polyline Vector will be sketched around the local area to be machined.

Ensure that the 2D View is active with the BitmapView switched on.
Select the Assistant tab.

Select Create Polyline
Create a closed vector around the eye and nose area as shown:

Select the vector in the 2D View.
Select the toolpathstab.
Select Machine Relief on the Toolpaths page.

Machine Relief will be applied using the Offset option to follow the selected vector shape starting from the centre outwards (Start Point – Inside).

Climb Milling is shown in Pink, and Conventional Milling is shown in Green when calculated.

Select area to machine as Selected Vector
Select an Offset strategy with an Allowance of 0.0, and a Tolerance of 0.01.
Set Climb Mill and the start point as Inside.

The Machine Safe Z and Home position are already set up.

Select a Conical0.25 Flat -15 Degrees tool from Steel  Engraving.
Edit the tool Stepover to 0.1.
Enter the toolpath name as Details.
Click Calculate Now and then Close the form.

The Offset finishing strategy is calculated by offsetting the selected vector inwards followed by reversing the order to start in the centre.

From the File Menu, select Save As and save in C:/Temp as training-my-ted.

There are now 4 toolpaths shown at the top of the toolpaths page.

This controls, which tool path is selected and what view it is shown in.

If a selected toolpath is double clicked, at the bottom of the toolpath page, an edit parameters button appears. Clicking this will allow you to edit the toolpath and calculate a replacement.

Simulating the Toolpaths

Generated toolpaths are simulated in the 3D view in ArtCAM. The simulation makes it easier to visualise the exact cutter path and surface finish, rather than the normal red lines used to display the toolpath. We can simulate the toolpaths in the order they would be machined to give as realistic a simulation as possible.

Select the Roughing Toolpath.

Click on the name roughing from the list so that it is highlighted and therefore selected.

From the Toolpaths page, click the Simulate Toolpath Fast.

The following dialog box will be displayed:

Relief Dimensions: shows the overall dimensions of the relief.

Simulation Block Dimensions: gives the size of the block. This should be at least as big as the minimum and maximum height of the relief plus any height (or depth) of the engraving features.

Simulation Relief Resolution: specifies the quality of the image that you require. Obviously the lower the resolution the greater the speed of calculation.

Select Standard from the Simulation Relief Resolution section.
Use the other default settings and click Simulate Toolpath.