The post New video shows Hybrid toolpath appeared first on Mastercam.
]]>Watch the video below to learn more.
Please contact us if you have any questions or try HSM Performance Pack by requesting a trial here.
The post New video shows Hybrid toolpath appeared first on Mastercam.
]]>The post Force machining at specified z-level appeared first on Mastercam.
]]>In the image below, toolpath on left is without forced machining and the toolpath on the right is with forced machining.
To specify fixed z-levels, you must select one or more points and set their Type to “Z-level”. The Z-coordinates of these points are then used as fixed z-levels in HSM Performance Pack. This option is available for Pocket3D, Contour3D and ConstantCut3D.
The post Force machining at specified z-level appeared first on Mastercam.
]]>The post HSM Performance Pack introduces new Drilling strategy appeared first on Mastercam.
]]>The new drilling strategy has been developed to provide users with specialized capabilities such as holder avoidance and rest machining. When using the drilling strategy, HSM Performance Pack can automatically analyse the part to avoid blind holes, gouges in linking moves and holder gouges if enabled. In the following we will look at some of the options available.
The new drilling strategy includes the holder collision detection policies Fail, Detect length and Trim that determine how HSM Performance Pack should react when a holder collision is detected. Fail ensures the operation always throws an error if a collision is detected. Detect length causes HSM Performance Pack to analyse the drilling toolpath and suggest a flute length that avoids any holder collisions. Trimming enables HSM Performance Pack to trim away the toolpath in collision areas and finally, there is also the option to simply ignore collisions if necessary.
Rest machining is another very useful option in the new drilling strategy that can be used in conjunction with the Trim collision detection policy described above. When Trim is enables holder collisions are avoided, but it might not be possible to drill all holes and to the desired depth. Rest machining makes it possible to easily run an additional drilling operation, with lower feedrate, that cleans out any remaining and unwanted material.
The option 3D Top is useful for pre-drilling angled and rounded surfaces which might cause the tool to slide or even break if drilled directly. With 3D Top enabled, HSM Performance Pack automatically creates the toolpath required to flatten the angled or curved area with a flat bottom tool.
Like all other strategies in HSM Performance Pack, the drilling strategy relies on STL models which enables it to work with any kind of part. However, it is essential that model geometry is made precise enough or this can result in some holes not being detected.
When an STL model is generated in Mastercam and made available to HSM Performance Pack as part of the normal workflow, we recommend using the following settings and even smaller tolerances can be used to increase the accuracy of the drilling calculations on the model.
If the STL model has been saved to a file, from Mastercam or other CAD system, the STL file can be loaded as Source Geometry – found under the Geometry tab. This can save time by not having to wait for Mastercam to generate the STL model repeatedly.
However, when loading an STL it is important to make sure that the tolerance used for the drilling operation is greater than the one configured in the STL model. We recommend that you double the tolerance for the drilling operation compared to the STL tolerance.
For those who wish to experiment with the new drilling strategy, a test part can be downloaded here.
For more information about the strategy, please see the Online Documentation.
The post HSM Performance Pack introduces new Drilling strategy appeared first on Mastercam.
]]>The post HSM Performance Pack 2020 publicly available appeared first on Mastercam.
]]>We are proud to announce the public release of HSM Performance Pack 2020 which is available for purchase as of today. We have spend the last five years developing HSM Performance Pack – our powerful add-on for Mastercam that offers highly specialized features alongside all the standard 3- and 5-axis functionality expected from any modern CAD/CAM system.
HSM Performance Pack includes an impressive set of machining strategies which are all built on our own new, state-of-the-arts, multi-core, 64-bit kernel. Every single strategy has been developed for maximum performance, flexibility and to accommodate customer requirements.
Every aspect of HSM Performance Pack has undergone extensive testing in real production environments and has been put to the test in shops, by our test users, for years. User feedback has and still is an essential part in shaping HSM Performance Pack and has resulted in custom and highly specialized features being built into the software.
HSM Performance Pack 2020 includes the following 3 and 5-axis toolpath strategies which can be fully customized in our easy-to-understand dialogs.
For more information about each of the strategies, please see our Features and Machining Strategies pages which also contain videos of each strategy. For detailed information, please see our online documentation, which describes each strategy and associated dialogs in detail.
HSM Performance Pack 2020 works with Mastercam 2019 or higher and requires you have licensed both Mastercam Mill 3D and Mastercam Multi-Axis. System requirements are similar to those of Mastercam and full details can be seen here.
Want to try HSM Performance Pack 2020? – then simply fill our the form here. If you have any questions then please feel free to contact us directly or request a callback.
The post HSM Performance Pack 2020 publicly available appeared first on Mastercam.
]]>The post Machining collapsed areas with Constant Cut appeared first on Mastercam.
]]>In the first image below, the collapsed areas are seen at the center of the rectangle and two circles. The second image shows the result of simulating the toolpath and clearly shows the wall remaining at the center of the rectangle.
To accommodate such situations, HSM Performance Pack includes an option “Ramp islands” which enables more accurate machining of collapsed areas. The option applies a ramping toolpath to the collapsed area which ramps down from above the stock wall clearing it out. It also ensures that the stock wall is kept thick enough so that it does not break while ramping.
In the image below, the option “Ramp islands” is enabled under the Milling parameters tab.
If more control is needed, ramp parameters such as Z-clearance, stepdown and angle can be configured in the Ramping section under the Linking tab.
With “Ramp islands” enabled and the ramping parameters configured, as shown in the image above, you get the following toolpaths.
When simulating the toolpath we can now see how a thicker stock wall is retained. This wall is then removed with the ramp starting at a Z-clearance above it and ramping down at a specified stepdown and ramp angle.
To try it out for yourself, download the example part “Constant Cut Islands Ramp Facing” which is also used in the images above.
The post Machining collapsed areas with Constant Cut appeared first on Mastercam.
]]>The post HSM Performance Pack introduces Hybrid Strategy appeared first on Mastercam.
]]>Users often prefer Contour3D for machining steep areas and Scallop or Parallel for shallow areas. However, this approach requires that several operations are created and that machining angles, contact boundaries and machining boundaries are configured. This is time consuming and often the ordering of toolpaths will not be optimal.
The new Hybrid strategy provides an alternative which is much easier to configure and that ensures optimal toolpath ordering.
The Hybrid strategy creates contour passes by default and lets the user configure an additional strategy (Scallop or Parallel) to use in shallow areas. Several machining modes are supported which can be configured by selecting the desired “Strategy”, for shallow areas, and a “Method” that determines where and how the strategy should be applied.
The Hybrid strategy is still in development with additional features planned before release. In the following we will look at the combinations, currently available, for setting “Strategy” and “Method”. In the configuration, options are divided into two sections – Steep and Shallow. The options in the Shallow section change depending on which “Strategy” and “Method” is chosen.
With these settings, HSM Performance Pack begins by automatically creating contour passes based on the specified stepdown value (Maximum stepdown). Only those where distances between passes does not exceed the Maximum stepover value are kept.
Next, using the contour passes as boundaries, the empty areas are “filled” with scallop toolpaths.
This approach results in all passes being closed unless trimmed for other reasons (boundaries, holders, etc.). The best result is achieved with parts that have a consistent Z value in shallow/steep areas which results in minimum variation in the XY distance between passes.
Image above: Setting Maximum stepdown and Maximum stepover values.
Image above: Contour passes which are kept. Empty areas will be filled with Scallop toolpaths.
These contour passes are kept because the maximum distance between passes, in the XY plane, is less than the Maximum stepover value. Contour passes are removed at the lower area towards the bottom because variations in the Z value at this point, due to the topology of the part, results in a greater distance between passes than allowed by the Maximum stepover value. The empty areas are then “filled” with scallop toolpaths as can be seen in the result below.
Image above: Resulting contour and scallop toolpaths.
With these settings, HSM Performance Pack uses the “Shallow angle” value to automatically define machining boundaries that determine in which areas contour and scallop passes are created.
It is recommended not to change the default 45 degrees “Shallow angle” value as this describes the best boundary value between shallow and steep areas. Scallop passes are created in areas with angles between 0 degrees and the “Shallow angle” value (45 degrees) while Contour passes are created between the “Shallow angle” value (45 degrees) and 90 degrees.
Image above: Shallow angle set to 45 degrees. Scallop toolpaths are then created in all areas with angles up to 45 degrees.
Image above: Resulting contour and scallop toolpaths.
With these settings, HSM Performance Pack uses the “Shallow angle” value to automatically define machining boundaries that determine in which areas contour and parallel passes are created.
Parallel passes are created in areas with angles between 0 degrees and the “Shallow angle” value. Contour passes are created in areas with angles between the “Shallow angle” value and 90 degrees. The option “Machining angle” enables users to specify the direction of the parallel passes.
Image above: Machining angle set to 0 degrees
Image above: Resulting contour and parallel toolpaths. All parallel passes are 0 degrees as specified.
These settings are almost similar to the above for “Fixed direction”, however, with “Method” set to “Automatic direction”, HSM Performance Pack automatically determines the best direction for the parallel passes in each area.
Image above: Resulting contour and parallel toolpaths with “Automatic direction” enabled. Notice that the direction of the parallel passes vary in different areas of the part. Compared to the previous image, showing “Fixed direction”, the direction of the passes on the left and right side have been set differently by HSM Performance Pack.
For examples of using the Hybrid strategy in HSM Performance Pack, please look at our demo part “Hybrid”.
The post HSM Performance Pack introduces Hybrid Strategy appeared first on Mastercam.
]]>The post Automatic angle detection with Parallel appeared first on Mastercam.
]]>This type of problem is easily solved with HSM Performance Pack. By enabling the option “Automatic angle” the optimal machining angle is automatically determined for every area – saving you lots of time.
Download our example part “Parallel with Automatic angle” to try it out for yourself.
“Automatic angle” enabled for Parallel under the Milling tab.
Parallel toolpaths with optimal machining angles.
The post Automatic angle detection with Parallel appeared first on Mastercam.
]]>The post Center passes for Scallop appeared first on Mastercam.
]]>Variation also occurs in areas where the toolpath gets collapsed and as a result the inner offset path becomes much smaller than the previous one.
The result of these variations becomes evident in the image below which shows a solid simulation of both toolpaths. Notice all the small red cusps inside the corners and in the collapsed areas. These cusps are all higher than what is allowed by the specified stepover.
Fortunately, Scallop in HSM Performance Pack includes an option called “Add center passes” which solves this problem and removes the cusps. The option is found under the Milling tab as shown below.
By enabling this, additional passes are added which goes through all the sharp corners of the normal scallop passes and through the collapsed areas.
The result of the solid simulation now looks much better with all the cusps eliminated by the extra passes.
To try it out for yourself, download the example part “Scallop star with center passes” used in the images above.
The post Center passes for Scallop appeared first on Mastercam.
]]>The post Toolpath control with boundaries appeared first on Mastercam.
]]>Boundary options in HSM Performance Pack include Machining, Contact an Stock boundaries which are supported by most of our strategies. However, the availability of these depends on the nature of the specific strategy being used. In the following we will have a closer look at these options.
For examples of using boundaries in HSM Performance Pack, please look at our demo part “Boundaries”.
As an example, the screenshot below shows the options available for our Parallel finishing strategy. Under the Geometry tab, a Boundary has been added in the “Boundaries and Points” section and the type of tool containment within this boundary is being set to Contact. Notice the options “Tool containment” which lets you control whether the tool is restricted to the inside of the boundary, can move to the center or move outside the boundary. This option is only relevant to Machining boundaries.
Machining boundaries enable you to restrict the tool to the inside, center or outside of selected boundaries by taking into consideration the radius of the currently active tool. Contours, that are selected as Machining boundaries, are not allowed to intersect and will cause an error.
Options for Tool containment include:
1) Inside: Keeps the entire tool (center + radius) inside boundaries
2) Center: Allows the center of the tool to move to boundaries
3) Outside: Allows the tool to move outside boundaries by a distance of the tool’s radius
4) Additional offset: Offsets the tool from boundaries by a distance. Positive value for outside and negative for inside
The offset value applies to all selected Machining boundaries and generates new, intersection free boundaries.
For roughing strategies, the selected boundaries are applied to the cutting passes which avoids having to use trimming and guaranties that any linking moves are also kept within boundaries.
For finishing strategies, cutting passes are trimmed against boundaries which ensures cutting passes are kept inside boundaries but linking moves might still be outside. Some finishing strategies further include the option “Follow containment” which forces HSM Performance Pack to apply boundaries to the cutting passes and ensure linking moves are kept within boundaries – similar to boundaries for roughing strategies.
Contact boundaries are used to ensure that the contact point between tool and surface are kept inside the selected boundaries. The main difference between Machining and Contact boundaries is that Contact boundaries lets you control the tool’s touch positions. Contact boundaries are primarily available and used with finishing strategies. However, the Horizontal strategy does not support Contact boundaries.
In the image above the red point indicates the contact point with the surface. The green point indicates the tool tip.
Please note that “Tool containment”, described above, does not apply to Contact boundaries.
Stock boundaries are normally used when specifying stock for roughing strategies with the option “Machining from outside” enabled, but it is also supported by the Horizontal strategy. It works similar to Rest machining and ensures that only cutting passes that touch the stock are kept which also avoids air cuts.
Please note that “Tool containment”, described above, does not apply to Stock boundaries.
The post Toolpath control with boundaries appeared first on Mastercam.
]]>The post Toolpath smoothing and simplification for Pocket and Horizontal appeared first on Mastercam.
]]>Fit Arcs is supported by most strategies in HSM Performance Pack including the Pocket and Horizontal strategy. Fit Arcs automatically splits the tolerance, defined by the user, and uses part of it for fitting arcs in slice passes. If this option is disabled, the resulting toolpath will only contains linear movements. In the screenshot below the toolpath on the left has Fit Arcs disabled while it is enabled on the right. The toolpath on the left has far more points since only linear movements are used to create the curved parts of the toolpath. On the right, the curved parts are converted to arcs which are defined by only a few points each.
With Minimum cutting radius arcs are fitted in internal corners to avoid the tool from making sharp turns. Minimum cutting radius is only applied to the outermost contour since otherwise, if applied to the whole toolpath, it could leave upstands on the part.
Maximum smoothing can be used to both smooth and simplify a toolpath to avoid sharp turns and reduce the number of points. Toolpaths which are smoothed are always inside the provided distance from toolpaths which are not smoothed. At the same time, the Stepover is automatically reduced to avoid upstands. This also means that the Maximum smoothing can never be more then the defined Stepover value. The outermost cut along the desired contour is never smoothed when using Maximum smoothing. This is to ensure that all material is properly removed.
The following screenshot shows a toolpath without smoothing on the left and on the right, the same toolpath with smoothing. Notice in the image on the right, that the stepover is slightly reduced when smoothing is applied, which can be seen by the additional cutting passes.
To avoid sharp turns on the entire toolpath a combination of Minimum cutting radius and Maximum smoothing is required. Minimum cutting radius is applied to the outermost passes while Maximum smoothing is applied to all other passes. In the following screenshot both options have been applied to the toolpath.
All smoothing and simplification options are located under the Milling tab and if you want to experiment with these options, you can download the file Horizontal smoothing from our Example Parts section.
The post Toolpath smoothing and simplification for Pocket and Horizontal appeared first on Mastercam.
]]>