3. Vectric Cut 3D

1 Orientate and Size Model

1.1 ‘Open’ to open a file

1.2 Top surface: Select ‘Top’

1.3 Model Size: Input the size of model with x,y,z dimension

1.4 Units: select according to your model. In this case, we use millimeter as the unit

1.5 Sides to Machine: Choose the number of sides to be craved

1.6 Click ‘Next’

2. Material Size and Margins

2.1 Material size: Input the length, width and thickness (x,y,z dimension) of the material

2.2 XY Origin Position: Set to 0

2.3 Machining Margins around Model: In this case, we set 11mm. The machine will remove the material in the area 11mm offset from the model.

2.4 Depth of Model below Surface: This step is for smoothing the top surface of the material. In this case, since the material we used has a smooth flat surface and the top surface of model is at the same level with the surface of the material, we enter ‘0’ in the box

2.5 Cut Plane Position in Model: This step is for setting the depth of material that we want to cut. In this case, we want to cut through the material, so we set ‘Bottom’. If it is the case of double side, you may need to set ‘Centre’

2.6 Click ‘Next’

3. Roughing Toolpath

3.1 Create Roughing Toolpath: Check the box

Click ‘Select’ to select the tool

3.2 Cutting Parameters:

Pass Depth: is the depth of cut in each pass. In this case, the material and model depth are 50mm and pass depth is 2.5mm, so the toolpath will make 20 roughing pass.

Stepover: This is the distance the cutter moves over when doing area clearance cutting. In this case, stepover is 5mm, so the grill will have 5mm overlapping with the cutting area in the previous move. The Stepover should be less than 50% of the diameter of the grill

3.3 Feeds and Speeds:

Spindle speed: In most of the cases, the spindle speed is 6000rpm

Feed Rate: Lower feed rate is suggested to set, like 30mm/sec. We can speed up the speed of mill after the process starts.

Plunge Rate: This is the cutting rate at which the cutter is moved vertically into the material.10 mm/sec is the average speed.

3.4 Tool Number: Set ‘1’

3.5 Toolpath parameters

Rapid clearance gap: 10mm is recommended. This is the height above the material the cutter will retract to when moving to different regions of the job.

Maching Allowance: 0.05mm is recommended. This is the amount of material to leave on the job when rough machining

3.6 Strategy:

Z level: The tool cut region by region of cutting area. The cutting time is shorter than 3D raster, but surface is relatively rough.

3D raster: The toolpath movements are parallel to the X,Y or Z axis

3.7 Side Displayed: Select ‘Top’

3.8 Estimated mc time

3.9 Click ‘Next’

4 Finishing Toolpath

4.1 Click ‘Select’ to select the tool

4.2 Cutting Parameter: In order to get a smooth surface, the stepover should be about 0.5 to 2mm

4.3 Feeds and Speeds: Refer to step 3.3

4.4 Tool number: Set ‘1’

4.5 Toolpath Parameters

4.6 Raster angle: It allows the cutting direction to be set parallel to the X axis, the Y axis or at 45 degrees.

Rapid clearance gap: Refer to step 3.5

4.7 Side played: Select ‘Top’

4.8 Click ‘Next’

5. Cut Out Toolpath

The Cut Out function is mainly for trimming. The drill will follow the outline of the model and cut.

Please mind that Cut Out function should not be used, if you don’t want the model separate with the material at the end. For example, the model has rib/bridge connecting to the edge of the material. If you use Cut Out function, the machine will cut off the model including the rib/bridge, so the model totally separates with the materal.

If you skip the ‘Cut Out’ process, uncheck the box of ‘Create Cut Out Toolpath‘ and click ‘Next’. If you want to process the ‘Cut Out’, please ensure that you checked the box of ‘Use Model Silhouette’ in the page of Material Size and Margins.

Page of Material Size and Margins

6. Preview Matching

The preview can be shows by clicking ‘Roughing Toolpath Preview’ or ‘Finishing Toolpath Preview’. The animation of the cutting process will be shown by checking the box of ‘Animate preview’.

If we set ‘Scale Factor’ as ‘1’, we will get the exact cutting time based on the setting in the computer. Since we may speed up the cutting rate after the cutting starts, the ‘Scale Factor’ should be larger to get a more accurate estimated time.

Click ‘Next’

7. Save Toolpaths

Select .txt format file in the ‘Post Processor’

Click ‘Roughing Toolpath Save’ to save the roughing toolpath file

Click ‘Finishing Toolpath Save’ to save the finishing toolpath file

Advertisements
%d bloggers like this: