DeskArtes
RapidCAM
User Manual
DeskArtes
RapidCAM User Manualfor Version 1
Copyright
Published by DeskArtes Oy, for release 1, Spring 1998.
© 1998 DeskArtes Oy. All rights reserved. No part of this publication may be reproduced, transmitted, transcribed, stored in a retrieval system, or translated into any language in any form by any means without the written permission of DeskArtes Oy.
DeskArtes Oy reserves the right to revise this publication and to make changes from time to time without the obligation to notify any person of such revisions and changes.
Trade Marks
DeskArtes, Rapid Tools, and the DA symbol are trademarks of DeskArtes Oy. Other brand and product names are trademarks and registered trademarks of their respective owners.
Contact Address
DeskArtes Oy
Kalevankatu 3 A
FIN-00100 Helsinki
Finland
Tel. +358–9–644335
Fax +358–9–644330
e-mail DA@deskartes.fi
URL: http://www.deskartes.fi/
Contents
Foreword
*About
RapidCAM *About this Manual
*Launching
RapidCAM *Principles of operation
*Tool path strategies
*Toolpath generation
*Toolpath coordinates and translations
*CAD Data
*Model requirements
*Hints for faster calculation
*Parts with undercuts
*Using
RapidCAM *Units
*Milling Process dialog
*Cusp height tolerance
*Minimum tool step
*Plate thickness
*Placement of the model
*Milling Parameters dialog
*Feedrate
*Spindle speed
*Plunge rate
*Rapid movement
*Lift height
*Safe height
*Options dialog
*Model type
*Postprocessing
*Advanced pocketing
*Optimize paths
*Tool selection
*Finishing tool
*Pocketing tool
*Guidelines
*Run Machining
*Inspecting the toolpaths
*
Table of Figures
Figure 1 From CAD-model to NC-code.
*Figure 2 Machining the first plate of a valve housing pattern.
*Figure 3 The first plate is machined and the machining of the second plate is started after joining it to the first one.
*Figure 4 The first two plates are machined.
*Figure 5 After the model is machined, the material frame is lifted away.
*Figure 6 The definition of the cusp height using a ball-ended tool.
*Figure 7 Relationship between step size and cusp height.
*Figure 8 The relation between the real lift height for a model built of 3 plates and the plate relative value given by the user. (a) - lift height for plate 1, (b) - lift height for plate 2, (c) - lift height for plate 3
*Figure 9 The toolpath generation with two different run modes. The so-called Core-box mode simply leaves the outmost boundary un-machined.
*Figure 10 Optimized toolpaths. The density of the toolpaths is higher in flat or near-flat areas compared to vertical areas.
*Figure 11 A ball-ended tool and a flat-ended tool with a sharp corner.
*
RapidCAM
RapidCAM
is a software that automatically calculates the NC-toolpath according to the STL data given to the program. The only interaction needed between you and the program is by means of dialog boxes for specifying the machining.Figure 1 From CAD-model to NC-code.
The standard machining features provided with RapidCAM include special milling sequences for flat areas and tool path optimization. Furthermore, RapidCAM
directly supports Layered Plate Manufacturing (LPM) techniques. Large models can be assembled by stacking plates and RapidCAM creates the milling sequence for each plate.
When RapidCAM is launched as a separate application, several menus are available for loading files, for viewing, and for applying linear transformations. These menus are not yet covered by this Manual.
This explains how to use the functions of
RapidCAM that are specific to milling. If you launch RapidCAM has a stand-alone application, only the MILLING menu is explained in this manual.RapidCAM
On Unix platforms, you can:
DA –C
DA –t –C
On Windows NT, a shortcut is created to launch
RapidCAM as a stand-alone application. If you wish to use RapidCAM together with the Industrial Design System, please contact your software supplier.This section explains the tool path strategies that are available in rapidcam, what sort of data is used as input, how the parameters are supplied, and, finally, what sort of output is generated.
Tools that exhibit la large length/diameter ratio are difficult to use. Another issue is the working area limitations of milling machines.
RapidCAM eliminates these problems by using a method of building the parts from plates that are joined together during the machining process.Traditionally, the working material is ordered in plate-like blocks, with a thickness of about 50 mm. The "plates" are then glued together to form a "cube", which is then rough machined and finally finish machined. As a result there is a lot of material that has to be removed.
When using
RapidCAM, you can machine the model one plate at a time. You can either machine one at a time and join them after the machining, or join the next plate directly on top of the newly machined one. The following shows an example of the latter method.RapidCAM
calculates the toolpaths one at a time for each plate and includes into the NC-code the required information (breaks) for performing a change of plates. After the toolpaths are generated the machining can begin. Figure 2 shows the machining of the first plate of a pattern for a valve housing. The plate thickness in the actual case is 20 mm.
Machining the first plate of a valve housing pattern.
Figure 3 shows the machining after the first plate is machined and the next is joined upon the first one. The plates can be joined together with, for example, a bonding agent. Once they are joined, machining continues.
The first plate is machined and the machining of the second plate is started after joining it to the first one.
In Figure 4 also the second plate is machined. While the desired shape is achieved, the milling machine works like a cutter of the plates. This means that the actual amount of removed material is a lot less than with the traditional method. The leftover material is simply removed with the material frame.
Figure 5 shows the machined model. Because of the positive drafting angles in the mold pattern, the material frame is easily removed in the end. The plates are separate to clarify their shapes. In a real situation they could either be joined together and be removed in one piece, or screwed together to simplify the de-assembly of the frame after machining.
Before toolpaths can be generated, you must supply several parameters. The parameters have been classified into four groups:
Once you have specified the values for each of the parameters in these dialog boxes, the toolpaths are generated when you select the Run Machining option.
The resulting toolpaths are stored in the named file you supplied to the Run Machining option with extension
.nc. In addition, they are loaded into RapidCAM for visual inspection.Interactive modifications to the toolpaths are not possible. To obtain new toolpaths, you must modify one or more parameters and generate them again.
The changes you make to the parameters in the dialog boxes are permanent. When they are displayed again, the last values you entered are shown even if you exit the program.
Toolpath coordinates and translations
The toolpath calculated by
RapidCAM probably does not contain the same coordinates as the original sliced CAD-model. This is because RapidCAM always moves the model in the coordinate system; in the z-axis direction so that the CAD-model is on the negative z-axis.To help the machinist,
RapidCAM outputs a file named after the output file, but with the extension .log, where the actual enclosing box is shown for the NC-file. Also the plate thickness’ and the machining parameters are found in that file.
CAD Data
RapidCAM
generates toolpaths using as input STL data. Consequently, if the CAD model is in IGES or VDAFS format, i.e. it is a surface model, it must first be triangulated.The 3D CAD model has to be either a closed surface model or a solid model. This is necessary in most CAD-systems in order to produce an STL file.
RapidCAM demands an error-free STL file to work correctly. Holes in the STL-model or overlapping triangles might cause problems.You can triangulate the model using the translator in
RapidCAM. The translator is available as an option to the basic package and it can be found under the Triangulate function in the TOOLS menu.If the STL data contains errors, these can be repaired by
RapidCAM using the Repair function in the TOOLS menu.
Manufacturing a model by milling always arises the problem of inner corner designing. The smallest corner radius that is possible to machine equals the radius of the tool that will be used while milling. Thus, fillet radius of an inner corner should be chosen at least as large as the tool radius.
Inner corner fillets with radii approximately equal to the tool produce time consuming calculations for tool compensation. If possible, the designer should use fillet radii that are bigger than the intended tool radius, and just leave the smaller ones out of the CAD-model.
Parts with undercuts
RapidCAM
does not support multiple setups. In other words, the part must be positioned such that surfaces to be milled are all visible to the tool at once. RapidCAM
It is assumed that, when applicable, values are expressed using the metric system, including the input data, tool geometry, speed limits, surface quality related values, and so forth.
The Milling Process dialog is the most important one in
RapidCAM because it includes the most important parameters.
Cusp height is defined from the tool geometry, according to Figure 6. It is the height of the stock material left in between two adjacent tool paths.
Figure 6 The definition of the cusp height using a ball-ended tool.
Defines the smallest step which can be used between adjacent toolpaths.
This value must be specified taking into account the desired cusp height and the shape of the tool. The best way to understand the relationship between these three variables is to consider the following Figure:
Figure 7 Relationship between step size and cusp height.
The shape of the cusp is a quadratic function. Small increases in the step size translate to sharp increases in cusp height. Likewise, small deacreases in step size translate to drastic improvements in cusp height.
A simple rule-of-thumb to determine what step size S to use for a tool of radius R and to obtain a cusp height H is to the following formula:
S = √(2RH)
For example, a cusp height of 0.01mm with a tool radius of 3mm requires a step size of about 0.24mm Since the formula does not take into account the geometry of the part, the suggested value should be decreased if the model needs good surface quality in near-flat areas.
If two adjacent toolpaths become too far apart, then the pocket milling tool will perform a pocket milling sequence in between the two toolpaths.
Using a small value will prolong the calculation time. But if the value is too large it is possible that the desired cusp height is not reached everywhere.
Therefore, we recommend the values of 0.05-0.2mm for the general case. Larger values, in the range of 0.1-0.3mm can be used with models or plates with vertical or near-vertical walls.
The use of plates for building large models is one of the main special features included in the
RapidCAM software. The program will automatically calculate how many plates are needed for the model.The physical thickness of a plate should never be less than the nominal. Otherwise there will be an area, on the upper plate, that will not be machined at all.
First the milling will happen in the air, and then when the next plate is joined upon the first, the milling will not reach the bottom of the plate. That is why we recommend to use plates that are just a fraction thicker than the nominal thickness. This has implications regarding the Lift height value.
The user can choose if the toolpaths are calculated so that the lowest point of the model will coincide with the bottom of the lowest plate to be used.
As an option, you can specify that the highest point of the model matches the top of the topmost plate.
Parameters that directly influence on the milling process are under this dialog. The values in this dialog box are influenced by the geometry of the tool, the milling machine, the material being cut, and the desired surface finish (not to be confused with cusp height).
The same values are applied when using any of the tools defined in the Tool Selection dialog box.
Specifies the feedrate during machining. The feedrate depends on the milling machine and the material that will be used.
The user can enter the spindle speed. The chosen value is dependent on the tool diameter, the feedrate and the material to machine.
Before a tool can cut away material, a hole must drilled. The plunge rate specifies how fast the tool drills the hole.
Tools used for machining soft materials do not often have good drilling abilities. In these cases, the plunge rate is quite small compared to the feedrate. Consult the Guidelines in the Tool selection section for more information.
The user can enter the rapid movement. The distance comprising of lifts and moves in the air, between the summits and valleys of a model, can be quite large. Moving these distances with maximum speed will lower the machining time.
If the APT postprocessor is chosen in the Options, this value becomes irrelevant. The code will just be written as
RAPID, and it is up to the APT translator to specify the value.
The user can enter the lift height. The lift height is the level up to which the spindle moves before jumping from one place to the next using rapid movements. This is a plate relative value. This means that the actual value is counted from the plate surface upwards.
For example, if the plate that is machined has its upper surface at -20 mm (in the milling machine coordinate system) and the lift height parameter has a value of 4 mm, then the real lift height will be given as -16 mm in the NC-code.
If the nominal plate thickness differs from the actual, there might be collisions during rapid movements, if the lift height value is too low.
Remember that the physical plate thickness can vary considerably from the nominal one. You must make sure that the lifts still will be above the plate surface, even when using plates that are thicker than the nominal one.
The user can enter the safe height. This is the level where the spindle (i.e. the tool) will move while adding the next plate, and before stopping the NC-program. The safe height must be a positive real value.
The model type can be defined as Normal (or Positive) or Core-box. The difference between both is shown in the next figure:
Advanced pocketing may be necessary if the model has flat or near-flat areas relative to the xy-plane.
Low corner machining
If the finishing tool has a corner radius different from zero and the bottom of the part is at the same level as the bottom of the first plate (see Model placement in the Milling Process dialog), then some stock remains due to the fact that the tool cannot move below the bottom of the first plate at the risk of colliding with the NC machine's platform.
If this option is set and the pocketing tool has a corner radius equal to zero, a separate toolpath will be created for this region using that tool.
If this option is Yes the density of the toolpaths is higher in low-gradient areas compared to high-gradient areas. This means equal surface roughness all over and faster milling.
Choose the right postprocessor according to the controller of the milling machine to be used. At the moment there are three different NC-language postprocessors available: Heidenhain, G-code (includes Fanuc) and Automatically Programmed Tool (APT).
The NC code is written onto a file with extension
.nc following the name you supplied with Run Machining command.
Tool selection
The user can select ball- or flat-ended tools separately for each one of the different operations, namely finishing and pocketing. A finishing tool is always required whereas a pocketing tool is optional but recommended.
The following values must be supplied for each tool:
If the diameter is set to zero, the associated tool is disabled. Therefore, you can disable the pocketing operations by setting the pocketing tool's diameter to zero.
A corner radius equal to half of the tool diameter defines a ball-ended tool. A corner radius equal to zero defines a flat-ended tool with a sharp corner. For a tool with diameter D, the valid corner radii R are 0 ≤ R ≤ D/2. A corner radius greater than half of the tool diameter is not allowed.
Figure 11 A ball-ended tool and a flat-ended tool with a sharp corner.
The cutting depth must be less or equal to the maximum cutting edge of the tool. Depending on the material, it may be necessary to restrict the cutting depth such that only a portion of the cutting edge is used.
The cutting depth of the finishing tool must be greater or equal to the slice thickness specified in the Milling Process Parameter dialog box.
If the cutting depth equals the slice thickness, several optimizations will not be done but it can prove usefull under certain circumstances. For example, you may wish to create quickly a rough approximation to the object using a relatively large step size. Alternatively, it can serve as a rough cutting strategy before five-axis milling takes place for the final finishing.
Pocketing tool
In flat or near-flat areas, adjacent tool paths become far apart. In these areas, a separate milling strategy called pocket milling can be used. This strategy is enabled when you specify a pocket milling tool in the Tool Selection dialog box.
If pocketing is needed but no tool is specified, unremoved stock will remain in the part.
Typically, the cutting depth of the finishing tool is less or equal to the cutting depth of the pocketing tool. For example, if both have a diameter of 10mm, the cutting depth of the finishing and pocketing tools might be 5mm and 7mm, respectively, if the material is soft.
The finishing tool is also used to drill the initial hole so that stock removal can begin. Ball-ended tools are usually worse than flat-ended tools for this kind of operation.
At the start of a drilling operation, the only point of contact between a ball-ended tool and the material is the tip. At this point, the rotational speed is zero, and the tool must be effectively pushed into the material. Flat-ended tools, on the other hand, usually have cutting edges at the bottom and the contact area is larger.
When all the desired parameters are given to
RapidCAM, the toolpath calculation can be started by clicking the Run Machining command. The program will start with an initializing process, continued by the actual calculation of the toolpath and performing the postprocessing in between the calculation of the toolpath for each plate.Before machining, the user should always check the toolpath correctness. This can be done in the graphical window of
RapidCAM.One element is created for each plate, and, for each plate, the toolpaths are classified according to their function.
Therefore, you can analyse the toolpaths for each plate separately, and for each plate, the different kinds of toolpaths can displayed separately too.