Ductboard Knife Setup

CAMduct has the ability to generate output files for many ductboard systems. The steps below walk through setting up a machine that has a trailing knife configuration, and generating the NC file that the table controller can read. The following tasks are covered in this topic:

Installing the Machine Setup

When ESTmep or CAMduct is installed, the files that control various machines are installed to the Database folder by default. This is typically located in C:\Users\Public\Documents\Autodesk\Fabrication <version>\Metric (or Imperial) Content\<version>\Database.

    When ESTmep or CAMduct is installed, the files that control various machines are installed to the "Database" folder by default. This is typically located in C:\Users\Public\Documents\Autodesk\Fabrication <version>\Metric Content\<version>\Database.

  1. Verify that the appropriate machine files exist in the appropriate location by clicking File Setup Installed Machines, or by clicking the Installed Machines Icon in the Utility Bar.

  2. If the cutting machine is not visible in the list on the Installed Machines dialog, add it to the list by clicking the Include button .

    This displays the Include Machine in Group dialog.

  3. Select the machine from the drop-down list, and click OK.

  4. Click Setup to display the Machine Editor dialog.

  5. The Machine Editor dialog contains a variety of tabs that define the settings used by the Installed Machine.

    Configure the choices on the Machine Editor dialog. First configure the Machine tab. The Machine tab contains the following options:

    1. The Name field lets you specify a name to identify the machine as it is displayed in the Installed Machines list.
    2. The Dimensions fields are where the physical table dimensions are entered. This is defined by the measurement along the Rail Axis, (Length), and the Beam Axis, (Width).

    3. Preset Points. The diagram below represents the table bed, and has a button in each corner. These are used to determine the key reference points on the table.

    4. Select a reference point and then click on the required corner.

    5. Origin: This is set to define the machine's x/y axis orientation and, in most cases the X=0, Y=0 point. This is machine/controller dependent and after installation should not be altered unless instructed by the software vendor.

    6. Home Point: This is the position where the software will place the Nested parts, if Move Nest to Home Point is selected in the NC Settings tab.

    7. Start Point: The machine will start to cut a nest from this point. If this is not the same as the Home Point, the tool will make a rapid traverse to the corner of the nest determined by the Start point.

    8. Park Point: This defines the position the tool will return to after the parts are cut, provided that the Go to Park Point, (4), option is selected. This lets you remove the cut parts and place a new sheet on the bed without the tool head getting in the way.

    9. Block Point: The Block Point is used in Level 1 installations where NC is written for a single part in the Profiler. The Block Point is a single point on the bounding rectangle of the part. The last line of NC would be a command to move back to the Block Point, so the same part could be cut again. If Go to Block Point (4) is selected then the tool will return here after cutting has finished. This is not used in the ductboard configuration.

    10. Nesting: Specifies a nesting position on the bed that may be different from the Home position.

    11. Go to Park Point / Block Point: If Go to Park Point is selected, the tool head will move to the location specified under the Park Point in Preset Points. The Block Point is not used in the ductboard configurations.

    12. Traverse Rate: (5) Enter the speed at which the tool head will move when in rapid traverse (between parts when not cutting) - typically 20,000 mm/minute or 800"/minute, but this should be verified with your machine supplier. This value is also used to accurately calculate the time to cut a sheet of parts.

    13. Dual Tables: Some machines can have two cutting tables, or are long enough to allow two sheets to be mounted along the length. The software can then be set up to move between tables automatically. This is currently not supported in the Knife configuration.

    14. Rip Cut: Before, or after, cutting a nest, the program can cut off any remaining length or width of the sheet, dependent on the settings here. A rip cut is a latitudinal or longitudinal cut that separates unused sheet from the part of the sheet that has been cut upon.

    15. If Rip Cut is selected, there are different ways it can be implemented.

    16. Along Rail Axis: Cuts the sheet along the rail length.

    17. Along Beam Axis: Cuts the sheet along the beam axis.

    18. To specify the type of cut (rail or beam) and the various options, once the appropriate rip cut box is selected, click Setup. This displays the following dialog, presenting the following options:

      Position: Allows the rip cut to be set either above nest or below nest.

      Cut Order: Allows the rip cut to be performed either before or after the rest of the nest has been cut.

      Follow part boundaries: Sets the rip cut to follow the outside of the parts on the nest allowing for the margin between nested parts. The following illustration shows how the rip cut follows the part boundaries along the rail axis.

  6. The next step is to configure the NC Settings tab.

    The NC Settings tab contains options that directly affect the final NC data file output.

    1. Move Nest to Home Point: This option will adjust the position of the nest to the Home Point specified in the Preset Origins.

    2. Apply Kerf: Applying Kerf within the software will adjust the NC to compensate for Kerf, nullifying the need to adjust it at the controller. This is Ticked in most configurations.

    3. Kerf Tight Gaps: This option will apply kerf to small spaces such as 3mm Vee Notches This is not used or needed in a Knife configuration.

    4. Keep Current Nest Part Order: If selected, the Post Processor will not change the cut order, if it has been previously edited on the Nest. This would not normally be needed in the knife configuration as cut orders are normally used for things like Heat Dissipation.

    5. Part Ordering: This option determines the order in which the parts will be cut. If the Keep Current Nest Part Order box is selected, this option will not be available. The Methods that can be selected are Label Application (i.e. keep the same cutting order as printed with the part labels) , Allow Heat Dissipation (not applicable) and Shortest Path (where the controller will make the decisions based on its own internal settings) . In a knife configuration this is kept at Label Application: Part

    6. Along Rail Axis / Along Beam Axis: This determines which axis is to be cleared first.

    7. Priority : These settings determine in what order the machine will use the tools to manufacture the parts.

    8. Part by Part: This option will use multiple tools on the same part before moving on to the next part. If this option is selected it will first cut with the Marking Tool, then the Groove Tool, then go round the same part with the cutting Tool. This can increase the cutting time if a sheet is full of small items due to the time taken to change the tools.

    9. Tool by Tool: On ductboard machines this will determine the order that tools are used in. Highlight a tool by clicking it, then use Move Up / Move Down arrows to change the tool order. It is recommended that the Tool by Tool option is used on a ductboard machine. The order normally used in the configuration would be Grooving, Marking, then Cutting.

    10. Simplify Islands: Simplify takes the drawing and reduces its level of complexity so that when the NC is written for it, there are less instructions to download to the cutting machine. This is not used on ductboard Machines or ductboard patterns.

  7. The next step is to configure the Controller tab where the post processor is selected, along with other parameters that affect the NC being written.

    1. Use Post Processor Library: In the ductboard configuration, we set the " Use Post Processor Library" to read the post processor supplied with the software. If this is not displayed, or available in the drop-down menu, click the Browse button and browse to the location of the post processor file, typically normally in the CAM-Duct folder. (If this is not available, contact your machine software supplier.)

    2. The default File Extension used by the router controller is automatically placed in the File Extension field. This can be edited, if desired.

    3. In the Motion section of this dialog, configure the following options:

      Most ductboard machines use code written in Absolute Mode. Ensure that this is selected in the Motion section of this dialog, or changed to Relative if so advised by the machine supplier.

    4. There is no need to enter a Machine Zero Offset.

    5. For NC Output Units, it is possible to convert the NC to Imperial (if working in Metric) or Metric (if working in Imperial), though this is not usually necessary unless the Main Database is not configured correctly.

    6. Conversion Multiplier: For the ductboard configuration, typically the Conversion Multiplier is set to 1. If working in Metric, the Decimal Places (NC Data) is typically set to 2. In an Imperial setup, this is typically set to 3. Your machine supplier will inform you if these values must be changed.

    7. Automatic Loading: if supported by the ductboard machine, this will automatically load the nest sheet number in the job after the first sheet has finished cutting.

  8. The next step is to configure the Remark tab. This tab allows you to place information into the NC code. This can be useful in reading the code by hand and tracking what is being done.

    1. Click Add arrow to move the desired information to be displayed from the Options column to the Use column.

    2. There is also the option to Suppress Remarks which will ensure that no extraneous information is written to the code.

  9. Next, configure the Special Features tab. In the configuration above, there are no Special Features supported by this Post Processor. Depending on the machine being used, the Special Features are specific to that machine.

  10. The Web Cut tab is not used in the ductboard configuration.
  11. Click OK to close the Machine Editor dialog.

This concludes configuring the Machine Editor tabs. The next task is to setup the necessary tools and tool behavior for this machine.

Tool Setup

To add and setup the tools for a machine:

  1. Access the settings for the installed machines by clicking the Tools button on the Installed Machines dialog.

  2. It is advised that the materials that are to be used are setup first by going to File Setup Main Database Materials, or by clicking the Main Database icon on the Utility Bar. This is because the tool settings will need to be configured to the different thicknesses of ductboard material to be used.

  3. Details on entering and configuring materials are available https://beehive.autodesk.com/community/service/rest/cloudhelp/resource/cloudhelpchannel/guidcrossbook/?p=FABRICATION&l=ENU&accessmode=live&guid=GUID-BEADE391-1DA7-4304-BF81-4FFF998DFA06.

  4. The Edit Tools dialog should be setup as above. If there are no tools in the setup, add them by clicking the " Add Tool..." button .

    This displays the available tools that the ductboard machine can support.

  5. Select the tools that are required so that the Edit Tools looks similar to the one above.

  6. We then have to setup the parameters for each tool. This is done by clicking on the tool name and then clicking the Setup button.

  7. The Tool Details dialog contains information on the tools used by the cutting machine.

    This dialog is split into 2 sections: Global and Details. Settings can be transferred from one to the other by using the Move Button.

    In the above scenario, clicking OK would move the Tool Diameter from the Global Settings to the Details.

    The following parameters are available on the Tool Details dialog:

    • Global Settings: These settings will be applied globally to this tool, regardless of the material being cut and the gauge of the material.

    • Post Number: This is used to identify the tools used by the machine.

    • Positioning Height: The Positioning Height is how far above the board the tool will move when traversing between cuts.
    • Diameter: This is the Diameter of the cutting tool being used, or in the case of the Knife tool, a value of 0.10 is used.
    • Plunge Rate: This is the speed that the cutting tool will descend into the ductboard material.
    • Details: The tool Details are the parameters that are Material and Thickness specific. These settings will be specific to the machine Controller and may vary between manufacturers. There are some controllers where these parameters are not used as they are programmed directly into the control. Some example details are as follows:
    • Material: This is the name of the material the settings are being applied to. This is automatically added to the tools database, and will list all materials from the Material Database.
    • Thickness: This is the gauge or thickness of the material, and is added automatically to the tools database from the materials listed in the Material Database.
    • Kerf Value : Kerf is the allowance required to compensate for the tool width. With thermal cutting tools, the kerf value is normally material and gauge dependent. If Kerf = 1.0, and you need a Part 100 x 100, then the program will compensate and cut along a center line at 100.5 x 100.5. When cutting a hole 100 x 100 the center line would be 99.5 x 99.5.
    • Extra Cut Through Depth: This is the allowance that makes the cutting tool cut through the foil and into the sacrificial MDF Board. This value may be variable but will be around the 1mm - 2mm mark. A couple of test cuts are normally required to find the optimal Extra Cut Through Depth.
    • Number of Passes: This is the number of times the tool will go round the cut path.
    • Feed Rate: This is the speed that the cutting tool will move through the material, and this will be dependant on the grade and thickness of the material being cut. By default, this is set to around 10000 but a number of test cuts may be required to find the optimal cutting speeds.

  8. Click OK to apply these settings and save them to the cutting tool database.

  9. The last tool on the list is the Null Tool which is used by the program, and does not need any settings.

  10. Click Close, then OK to close the machine database.

This concludes setting up the tools on the machine. The next step is to set up the pattern options for ductboard in the pattern database. See Ductboard Database Pattern Options Setup below.

Ductboard Database Pattern Options Setup

Once the machine has been setup, the next step in Ductboard Knife Setup is to define the parameters within the Pattern Database Pattern Options DuctBoard.

A number of differnt types of system exist that utilise different cutting and marking techniques for creating duct from this material. To satisfy and select the requirements of each specific type of machines, select options in the "ductboard" section of the Pattern Database dialog. The ductboard database lets you customise settings to match specific tools and settings for each machine type.

Choose Machine

This lists the available machines setup on your system. It takes this information from the machine Database, along with any relevant tools that have been applied.

The next section determines the tooling and length of any marking and fold indicators. This is split into the type of fold, Radial (As used on a Radius Bend Back Wrapper) or Angled (as used on a Rectangular Bend Back Wrapper), and whether the fold is on the top or bottom of the material.

The Bending section specifies how many fold lines to place on a Radial Fold, or what spacing to use on the Radial Fold.

The Seaming Section specifies to use the Default Grooving Tool to apply the Seam Chamfers, or to specify what tool, from the available tools in installed machines, to use when cutting or Marking Seam Edges.

Parent topic: Installed Machines