[ddgman2001]

I don't quite understand some of the features of VM5 that are not included with the basic version. Could someone please esplain some or all of these features?

Re-Machining

Pencil Tracing , including Flat Mills

Valley Re-machining, along the cuts

Curve Machining

Spiral Machining

Radial Machining

Between 2 Curves Machining

Reverse Post Machining

Horizontal Hill Machining

[senor J.]

trying to get questions answered on this forum is difficult

[nervis1]

I can help with a few, pencil is a tool path that takes a smaller cutter to the edge between two surfaces to clean out the edge after a rough pass with a bigger cutter. Re- machining is a semi finish or finish pass using a smaller cutter to avoid air cutting in finish passes. The smaller cutter will just cut the areas not cut by the bigger roughing mill.

Radial starts from some location and radiates the tool path in angle steps, usually used for circular (think frisbee shape) projects.

[ger21]

http://www.ctsx.com/visualcadcam/whatitcando.html

[DareBee]

ddgman2001

You have asked for a HUGE pile of info.
Sorry but I am NOT about to type all of that out.
Here are excerpts from the VisualMill 5 help files.
Hope this helps some.

Pencil Tracing* : Roughing or finishing to cleanup valleys
This type of milling can be used either as a roughing toolpath or as a re-machining or cleanup toolpath. Here the milling cutter is driven along valleys and corners of the part geometry. The system finds all of the double contact or bi-tangency conditions on the radius on the given tool and drives the tool so that these areas are machined. Used as a roughing operation, this operation relieves valleys and corners of the part so that subsequent operations will not encounter large amounts of material found in these regions and thereby reducing tool deflection and wear. Used as a cleanup operation, this removes the scallops typically left along valleys by finishing operations.

Radial Finishing* : Re-machining annular regions
Radial Finishing is a toolpath method which can be used as a finishing operation for regions that have annular pockets. In this toolpath method the user has to specify one or more enclosed areas as the machining region. The pattern of these linear cuts can be defined by the user to be either Zig or ZigZag. The system calculates the centroid of the active region and generates the radial toolpath.

Spiral Finishing* : Re-machining circular regions
Spiral Finishing is used to generate toolpaths in regions that have circular or near circular characteristics such as pocket bottoms. The user must activate single or multiple machining regions to generate the spiral toolpath. The system analysis the region and calculates its centroid to be used as either the start point or the end point of the toolpath as specified by the user.

Curve Machining* : Machining on a closed curve
The Curve Machining operation allows machining along a closed curve. It is especially suited for engraving. The user must define and activate the required regions and can specify the direction and the pattern to be followed by the cutter.

Between 2 Curves Machining *: This toolpath method allows machining between two user-defined curves. These can be open or closed curves. The user can select machining to be performed either parallel or normal to these curves. The created toolpath will make a gradual transition from one curve to the other depending on the geometric form of the two curves. This creates a blended toolpath that can be used to efficiently finish complex shapes. This type of machining is sometimes called Flowline machining.

Reverse Post Milling*: Read previously generated programs
Reverse Post Milling can be used to read in existing G-Code or APT CL files and generate cutter paths. These cutter paths can alterntatively also be used to drive a cutter to machine part geometry.

Valley Re-machining* : Re-machining valleys in areas where a large cutter could not reach
Valley re-machining is used to machine areas where the tool used in a previous finishing operation was unable to access material. This typically happens in the valleys and corners of the part geometry. In this toolpath method, the user specifies two tools, the first one being the tool used in the prior finishing operation and the second smaller tool to re-machine the areas where the larger tool could not get in. The system automatically calculates these inaccessible areas and creates a re-machining toolpath.

Plateau Machining* : Finishing areas that are flatter than an angle
Plateau re-machining toolpaths are used to machine the tops of flat regions. The flat regions are defined by an angle from the horizontal. The system analyses the part geometry and determines all regions that are flatter than this user defined angle. Then toolpaths are generated to machine only these flat regions. This method of re-machining can be used to re-machine the areas that might have not been completely machined by a Horizontal Roughing or Horizontal Finishing toolpath.

Parallel Hill Re-machining*: Re-machining areas steeper than an angle using contour machining
Hill re-machining is used to machine steep areas in a part. The hills are defined by an angle from the vertical. The system analyses the part geometry and determines all regions that are steeper than this user defined angle. Then toolpaths are generated to machine only these steep regions. The system also automatically adjusts the cut angle so as to always machine "normal" to the steep areas, thus leaving as little scallops as possible on the part. This toolpath strategy is used when a Contouring Finish toolpath leaves larger than expected scallops on the steep areas of the part.

Horizontal Hill Re-machining*: Re-machining areas steeper than an angle using horizontal finishing
Hill re-machining is used to machine steep areas in a part. The hills are defined by an angle from the vertical. The system analyses the part geometry and determines all regions that are steeper than this user defined angle. Then toolpaths are generated to machine only these steep regions. The system also automatically adjusts the cut angle so as to always machine "normal" to the steep areas, thus leaving as little scallops as possible on the part. This toolpath strategy is used when a Contouring Finish toolpath leaves larger than expected scallops on the steep areas of the part.

[brtlatjgt]

this:

http://www.mecsoft.com/Mec/Downloads...esentation.htm



Note: Use Internet Explorer. Firefox wont open it.

[ddgman2001]

Thanks for those explanations. That's cleared things up quite a bit.