The CAM GRAAL 3D module is a software program for calculating tool paths on 3D surface geometries with a view to carrying out 3D / 3 axis milling on your Charlyrobot.

CAM GRAAL 3D generates tool paths in preform and / or in finishing with different strategies optimising the production and quality of the parts created.

CAM GRAAL 3D offers you, as on the 2D / 2D1/2 version, a simple intuitive method of setting the path parameters by successive windows with automatic or manual choices, and according to your choices, the optimal tooling values will be proposed to you.

You have among other things the tooling simulation module in realistic rendering.

The CAM GRAAL 3D software enables you to machine either surfaces made on the CAD GRAAL surface drawing module or surfaces from all the 3D surface or solid modelers capable of generating files in "STL" format.

The " STL " files will be imported first of all into the CAD module in order to make any modifications: (direction, size, Etc.) then transferred into the CAM GRAAL 3D module.

The files created in the CAM GRAAL 3D module will be saved with the extension : "*.F3D "

You will find in CAM GRAAL 3D all the general functions of the CAD (Zoom, change of views, copy / paste, Etc.)

Certain functions of preference are however specific to CAM GRAAL 3D (trajectory, approaches, Etc.)

The selections of the surfaces can be made in perspective views or in any views.

To help you start using CAM GRAAL 3D we propose that you make a simple example in order to understand how the software works; we will then propose you machine the 3D exercises that you have made in CAD.

You will first of all draw any surface in the CAD module, following the instructions in the manual (for example make an extruded surface as on the following image)

In CAD you can determine manually the workpiece necessary to create the piece. As it happens, for this example, it would be sufficient to increase the " Z " dimension then to make a movement of the surface inside the blank.

But as CAM GRAAL 3D has an automatic blank calculation function, we will for this example use this.

From the CAD, click on the icon " FAO3D " 

You switch automatically into the CAM module and the window " dimension and type of material " appears.

In this window, you will first of all choose the material that you will machine by scrolling down the list.

You will then reframe the dimension of the blank according to the dimensions of the surface to be machined. This reframing is made with margins at the top and the bottom and on each side, whose default values are 10 mm on all the sides except on the top where it is 1 mm (these values can be modified in the preferences.)

Scroll down the list of materials and choose " Labellite foam "( Labellite foam is a very tender material to machine designed validate shapes. This product is available from our list of accessories).

Click on " automatic reframing " and validate with: " OK ".

You are now in the CAM GRAAL 3D module in perspective view.

Select the surface by clicking on it, it will go into selection color (red / pink) and will be surrounded by a parallelepiped of selection.

Click on the right button of the mouse to call up the contextual menu, and click on: " describe the machining ".

You must in the first window specify if you are making a path in " Preform ", in " Finishing " or both.

The most usual rule is to make a " Preform + Finish ". In fact, in 3D / 3axes machining, the machining heights of the " Z " axis are often considerable and the finishing cutters only rarely have the possibility of carrying out the machining directly, so a preform cut with a specific cutter is very often necessary.

Click on: " Preform " then on " Finishing " then on " next "

The following window asks you to choose a preform tool from the list of tools supplied with the software.

Click on: tool N° 17 " cutter 2 flutes of 6 long " then click on " next ".

You must then choose the finishing tool.

Click on: tool N° 18 " ball cutter of 3 " then click on " next ".

Once the tools are chosen, the following window proposes you choose the preform machining strategy.

If you choose the " automatic " mode, a default strategy will be adopted and you will not have access to these parameters; you will therefore go directly to the window " finishing machining strategy« ; the automatic mode is particularly advised for users who are beginners in 3D machining.

If you choose the " Manual " mode you have to set your own parameters for the preform tool path in the following window.

Thi s window also shows you the depth of cut that will be generated with this tool in the material chosen. You can if necessary modify this value if the tool or the material used differs from those chosen from the lists, in all cases the advised value remains indicated in the information.

For this example, you will use the " Manual " mode so as to add comments to the window : " manual test strategy ".

Click on the button " Manual ".

The following window will enable you to choose the test strategy (it displays by default the strategy adopted in " automatic " mode.

First of all, you can choose between two methods : " Z constant " or " deep cut ".

The " Z constant " consists of making a path on parallel plane by going round the areas of the surfaces ; the depth of run will be determined automatically according to the tool and the material.

" Deep cut " consists of making a return scan following the profile of the surface with several cuts. As for the first method, the depth of cut will be determined automatically according to the tool and the material.

The finishing of the preform contour consists, it it is selected, of going round at each cut the preform islands of the surface (this function is only active in the " Z constant " method).

The allowance is the thickness of material left by the preform for the finishing, by default: 0.5mm.

The choice of scan indicates the axis in relation to which the machining will take place, either the " X " or the " Y " axis with an angle to be entered; the default scan is in relation to the " X " axis.

The scan increment is the distance of movemrnt of the tool at each cut; it is a percentage of the tool diameter, by default: 50°.

The tolerance / real surface is the admissible approximation between the drawing and the tool path generated; by default it is: 0.1mm.

For this example, you will leave the default values and click on " next ".

As for the preform, the following window asks you to choose a finishing strategy, either manual or automatic; the only difference : in automatic mode, you will choose a quality of machined surface with three options: " fine ", " medium " or " rapid ". In fact, these options correspond to the value of the scan increment , which, if it is very close, will give a very smooth surface,and conversely, if it is less close, will give a more or less rough surface.

As the value retained is the height of the crest generated by the action of the tool between two scans, then according to the tool and the surface, the increments can be different for a same crest height.

The default crest heights for the three options are:

- Fine : 0.01 mm.

- Medium: 0.05 mm.

- Rapid: 0.1 mm.

For this example and as for the preform, you will use the " Manual " mode so as to complete details in the window: " manual finishing strategy ".

Click on: " Manual " then click on " next "

8.5 Description of the finishing strategies

The machining method can be made by the following scan: X or Y or following an angle to be entered; it can also be carried out in " concentric " mode, in other words by describing a path turning round the surface; the default method is a scan following: " X ".

The " crosswise locating point " function, it it is activated, makes it possible to restart the machining after the first cut in places on the surface where the basic strategy has not managed to give the desired result; these areas are calculated automatically.

The restarts are by default carried out in automatic mode perpendicular to the basic strategy but can be chosen manually: following: X or Y or following an angle to be entered.

The " no variable machining " function enables the scan increment to be adapted to the slope of the surface in order to have as regular a result as possible; in fact, the closer the slope is to the horizontal, the closer the increment and vice versa.

The crest height (explained above) can be adjusted manually in this field; by default it is: 0.05 mm.

The tolerance / real surface is as on the preform the admissible approximation between the drawing and the tool path generated; by default it is: 0.05 mm.

The " allowance ",if you give it a value greater than " 0 ", then enables a new superfinishing path to be made with another strategy and / or another tool, the default value is: " 0 ".

For this example you will leave the default values and click on " next ".

The following window proposes you visualise or not the additional parameters; if you click on " next " without selecting " show the additional parameters ", you launch the path calculation immediately. On the other hand, if you select this command, the following window will ask you to enter these parameters!

If you only make very simple machining paths and never use the additional parameters, you can choose not to display this window at all and thus launch the calculation immediately after the window: " Finishing strategy ".

To deactivate the box asking for advanced parameters, you must open the preference sub-menu of the display menu then choose the tab: " Advanced " then the button: «global " and finally: deselect the function: " show the dialogue box: advanced parameters ".

For this example, in order to present you with all the functions, you will visualise the additional parameters by selecting the button.

Two parameters can be entered in the following window that we will comment on here:

This function consists of giving a limit to the area to be machined. In fact, by default the material is removed all round the surface on the whole of the blank, but if you are drawing in 2D any contour around the surface (which can be the edges of this same surface) and you select this contour with the surface to describe the machining, the fact of activating the restriction area will limit the machining on this contour (the tool can be stopped either in the centre or inside this contour).

If your drawing includes several surfaces and not all of them are associate tool paths, the areas of these surfaces can be avoided if you select this function.

Click on " next to launch the calculation.

A scroll bar as well as a message bar indicate the progress of the calculation. For this example, taking account of the simplicity of the treated surface, the calculation will be relatively rapid; but depending on the complexity of the surface(s) and strategies adopted, the calculation times can be more or less long ( several minutes or tens of minutes!)

Once the calculations are complete, a window indicates all the parameters of cuts as well as the estimated times for machining in preform and in finishing. These parmeters have been calculated according to the material and the tools used. If necessary you can make modifications and therefore recalculate the estimated machining times.

Once you have clicked on " finish» you can visualise the tool paths that you have just created. These paths are selected by default, and you can if you wish make modifications to them by clicking on the right and choosing either the menu: " Modify the machining » which scrolls for you all the windows from first to last, enabling you to make all the modifications you wish (this function, even if no modifications have been made, recalculates the paths); or the menu: " Modify the parameters » which like in the CAM 2D proposes that you choose to open one of the six windows and modify only that one. (in this case, some modifications which do not affect the geometry of the path do not cause its recalculation).

Once the paths have been deselected, you can visualise the preforms in red and the finishings in green.

N.B.: to create these paths you have openend all the available windows with the aim of knowing them; so we advise you to delete the paths that you have just created and restart the description of the machining by using the automatic functions to appreciate the speed and ease of use of the software.

Once the paths are made you can visualise the machining simulation on the screen with a representation in realistic rendering.

Click on the icon: simulation

Once you are in the simulation module, you can choose the direction and if required the size of the simulation with the " zoom " mode (these manipulations are made in line mode for more comfort).

The choices made, select the " realistic " button then the green button to launch the simulation.

You can now machine the surface that you have just created by clicking on the icon " machining " . ATTENTION : if you have used the automatic reframing function, the dimension of the height of the blank will have to be modified in the control module according to the actual thickness of the blank.

Click on " machining " and follow the instructions already seen in the 2D machinings taking care nevertheless with the tool outlets which absolutely must be higher than the maximum height of the surface to be machined.

The Approaches

The parameters of the tool approaches to the material to be machined are default set in the " preferences " sub-menu of the display menu. Depending on the strategies adopted, the approaches can change:

In vertical plane machinings, you can use either a vertical approach, or a normal approach to the surface, with the possibility of setting the parameters of the length of the approach vector.

In concentric machinings, you can use either a vertical approach, or a circular approach with an approach radius whose parameters can be adjusted.

The STL files are a complete representation of the piece, so some parts cannot be machined (concealed hollow parts, undercuts).

To ease the calculations, you can ask the software to take into account only the facets that have positive or neutral normals.

The parameters of this function are set by default in the " preference " sub-menu of the display menu, then in the " global " button of the tab " advanced ".

The machining record reminds the operator of all the parameters used for the machining(s). It also enables the machinings of the different paths to be sequenced.

This lrecord is displayed on the left side of the screen by clicking on the icon: " record "   but it is also displayed before the simulation and the machining.

The machining record can be printed.