Cut a single surface by following flow lines that define the surface. A set of splines that flow in two directions define the surface. These splines form two sets of flow curves. The surface arrow that is attached to the surface points toward one set of flow curves.
The direction of the Cut operation is toward the surface arrow. Change the direction of the surface arrow with the Edit > Surfaces > Direction command.
The Project operation projects an existing toolpath on a surface to create a new toolpath. The Project operation can be done in 3, 4, or 5 Axis machining.
The toolpath that is projected is normally created on one design and projected on another design. The tool moves in the projected toolpath can exist at different depths. These depths are kept on the new design after the toolpath is projected.
|
Project a toolpath on a number of surfaces |
|
|
Before |
After |
|
|
|
Begin The Project Operation
The Project operation requires some preparation.
There
are two requirements for the successful performance of the Project
operation.
A. One file must contain both the projected toolpath and the surface
on which that toolpath is projected. If these two items are in different
files, use the Append option on the Open dialog box to merge the two files.
B. The projected toolpath and the surface on which that toolpath is
projected must have the correct position. Use Edit
> Transform to change the position of the
surface. Use the Transform Operation button
on the Operations Manager dialog box to change the position of the toolpath.
Click Project on the NC > 3, 4 or 5 Axis menu.
The prompt tells you the select the surfaces. Use the Select menu to select the surfaces onto which the toolpath is projected.
After
you select the surfaces in 3 Axis or click OK in the 4-5 Axis, the Select NC Operation dialog
box appears.
From this dialog box you select the toolpath that is projected.
Click the icon of the toolpath to project on the surfaces and click OK.
After you click OK, the Project dialog box appears. Set the dialog and click OK.
Z Rough removes a large amount of material to prepare for other operations. The operation uses 2 axis (XY) tool moves in Z increments.
SURFCAM displays the Select menu. A prompt tells you select the surfaces to cut.
After you select the surfaces, the Material Information dialog box appears. Use this dialog to describe the part material.
The Plunge Rough operation quickly removes a large amount of material. Plunge Rough removes the material with feed moves in Z only. A series of overlapping plunge moves are made that remove cylindrical plugs of material. The axial strength along the machine tool spindle allows for high feed rates than can be maintained with XY moves.
Plunge Rough Tools
The tools that are used to do the Plunge Rough operation are rigid and have cut edges at the face. These tools cut the material only in the Z direction. The tools cut the material at a high feed rate. There are two types of plunge rough tools.
Center Cut Tools
Center cut tools can cut with the full diameter
of the cutter face. The first plunge cut tool move in the toolpath is
done at a decreased feed rate. The decreased feed rate is required because
of the slower cutter speed near the tool center. The next plunge moves
have increased feed rates.
Non Center Cut Tools
A non-center cut tool does not remove the
material at the center of the tool. A post of material is left at the
center of the plunge location. The next plunge move must cut this post
of material. These tools can cut at higher feed rates than other tools.
When you click Plunge Rough, the Select menu appears and the prompt tells you to select the surfaces to cut.
Select the surfaces to cut and click Done to see the Material Information dialog box.
Boundary Type identifies either the material boundary or the boundary of a tool containment area. The Boundary Is parameter controls how the Boundary Type is used.
The Z Finish operation cuts multiple surfaces by using a 2 axis (X,Y) contour cycle, but in Z axis increments. The Z Finish operation is most efficient at cutting surfaces or areas that are steeper or closer to being vertical, such as the following.
The Z Finish operation can cut nested boundary curves. The nested curves function like pockets that have islands.
SURFCAM always cuts the inside of the outer boundary and does not cut any islands that are inside this boundary. This method gives the ability to Z finish the outside of a part and only the outside. To cut only the outside of a part, use two boundary curves. Use one large curve to contain the complete part and a curve that is inside of that curve. The toolpath keeps away from the second curve.
Create toolpaths over multiple surfaces. There are two types of Planar operations: Planar Type and Flow surface.
The Planar and the Flow Surface operations have tool containment features. These features let you put a limit on the areas of the surfaces to cut.
See Check Surfaces on the Planar Cut Control tab dialog.
When you click Planar, the Select menu appears and the prompt tells you to select the surfaces to cut. After you select the surfaces, the 3 Axis Planar dialog box appears.
|
The SteepShallow operation lets you cut steep surfaces and shallow surfaces as one operation. Or you can turn off steep or shallow cutting. This gives you the option to cut steep and shallow surfaces with different tools, as separate operations. Since the tool engagement for steep or shallow cutting is steady, you can maximize the speeds and feeds. You can also control the overlap between steep and shallow cuts, for a smooth transition. |
|
|
|
|
|
3D Offset finishing is available only with the 3Axis Plus option. The 3D Offset operation allows 2D or 3D boundaries, and creates concentric, offset cutting passes. The shape of the cutting passes matches the shape of the outer contour of the part. The 3D Offset operation measures the step Increment three dimensionally on the selected surfaces. |
|
Some of the benefits of 3D Offset finishing are as follows.
· The toolpath maintains a constant scallop height, for a consistent finish.
· The tool can climb cut or conventional cut throughout the toolpath.
· Steady tool engagement accommodates maximum speeds and feeds.
· Cut from the outside in, or from the inside out.
|
Click NC > 3 Axis > Flat Surface. You can select all surfaces and the Flat Surface operation cuts only those areas that are perfectly flat. The Minimum Area setting lets you exclude flat areas that are too small. This value determines what areas are too small to cut, and the tool path ignores those areas. |
|
Contour 3D also appears on the NC > 2 Axis menu. See NC 2 Axis Menu.
Drill also appears on the NC > 2 Axis menu. See NC 2 Axis Menu.
Pilot Hole also appears on the NC > 2 Axis menu. See NC 2 Axis Menu.
Auto Rough removes large amounts of material from around a part by using a 2 axis (XY plane) cutting cycle at incremental Z level depths. Auto Rough is designed to work ONLY in Top CView.
Use a Planar (
) operation to guide the Auto Rough
cutting operation. You could use toolpaths from a Cut
operation or a Z Finish operation. But, because
the tool moves from a Planar operation are
linear and parallel, as viewed from top view, they provide the most efficient
guides for Auto Rough cutting.
|
A toolpath Auto Rough can use
|
Auto Rough operation
|
When you create this Planar operation, you must set parameters on the Tool Information and Cut Control tabs to meet the needs of the Auto Rough operation. On the Tool Information tab, use the same tool that you use for the Auto Rough operation. On the Cut Control tab, use the same value for Stock To Leave and you set Step Type to Increment.
When you click Auto Rough, the Select NC Operation dialog box appears. Select the Planar operation.
Rest Material removes the material remaining after all the operations in a single Setup.
The Rest Material menu appears and the prompt asks you to "Select Operation for Rest Machining."
All the Setup Section operations, as well as the Rest Material operation itself, must be performed in Top CView.
If there is only one Setup in your project, SURFCAM performs the Rest Material operation on the material left over from all the operations in that section. If there is more than one Setup Section, SURFCAM prompts you to select the section on which to operate.
Pencil Cut removes material left by previous operations along the concave intersection of two surfaces, or material left in "crease like" regions in a single surface.
SURFCAM calculates "pencil curves" along the uncut areas. Pencil curves are similar to the cutter intersect splines created with the Create > Spline menu.
To calculate a pencil curve between two surfaces, an offset from each surface is first calculated. The curve representing the intersection of these offset surfaces becomes the pencil curve. These offset surfaces are determined by the Tool Diameter and Tip Radius of the tool you elect to use to perform the cut.
When the tool is a ball nose, the offset surfaces are those that would be traversed by the center of the ball nose. The resulting pencil curve would be the curve traversed by the center of a ball as it rolls along the intersection of the two surfaces. (In the interior of a single surface, pencil curves are created in those regions that are so concave that the ball can contact the surface in two locations at once.) In similar but more complex ways, offset surfaces are created for bull nose and end mill tools.
The Pencil Cut toolpath consists of a single traverse of the tool along a path guided by each of these pencil curves.
Normally, in order for the Pencil Cut operation to remove material, a tool must be selected that has a diameter less than the one used in the previously performed operation.
From the menus, click NC > 3 Axis.
Tool Information Tab
for all mill operations.
