Overdrive
Pro Tool File Tools Tab
The “Tools” list-box groups the tools into four different categories: vertical drills, horizontal drills, routers, and saws. As you select radio buttons, the tools falling into that category will be displayed. You can add and delete tools by using the two buttons below the list box. Once a tool is selected, you can modify any of the properties of that tool. To save the changes once properties of a tool have been modified, click the “Apply” button located in the lower right corner of the screen. If you are working in Imperial inches, enter the values in inches. Otherwise, enter the values in metric units. If you fill out a tool file in one unit of measure and later change the unit of measure you are working in, the values will be automatically converted for you. Most of the properties are self-explanatory; however, details about some of them will be covered below. Default Depths You can assign a list of default depths for each tool in the tool file. As you will discover when you apply machining to a panel, you do not have to type the depths over and over again because a list of available tools and their drilling, routing, or sawing depths will be provided. In this box, enter the drilling depths you commonly use. For vertical drills, it is only necessary to enter one set of depths per diameter. If you do not fill out any default depths for a tool, that tool will not become available to use while applying machining to a panel. Multi-Pass Tool Functionality It is common to make multiple passes at different depths to accomplish a desired machining operation. Having multiple entities in AutoCAD on top of one another makes editing difficult. For this reason, the tool file allows you to set up special router tools that make multiple tool passes. The “900 Tool” is a “virtual tool” used in assigning more than one tool to the same tool path. The tool is actually a macro that applies one or more tools to a defined tool path. For example, if you would like to route a circle with one tool and then fillet the top corner of that routed circle with a different tool, you would use the 900 Tool. All multi-pass routers are numbered between 900 and 999 inclusive. You probably do not actually have a tool name “900” on your CNC controlled equipment. Instead, it is a designation the software recognizes as a combination of specific tools, depths, and offsets. There are two basic conditions for which you might want to use the 900 Tool: 1) Multiple passes of the same tool, or different tools in the same path, to a final depth as specified. The amount of material removed during each pass is a calculation of the final depth divided by the number of passes specified. These are called “Stepped Passes”. 2) Multiple tools in the same path (these can have different offsets if desired). To set up the 900 Tool, select the “Routers” radio option button from the "Tools" tab. Either select an existing 900 series tool or click the “Add New Multi-Pass Tool” button. There are two types of multi-pass tools you can use. Select the appropriate radio button to make your choice. “Multiple tools” enables a single routing path to be done at different depths with different tools. This option would apply if you need to cut a groove with a straight cutter and then go over the same path with a round-over cutter. A “Step” multi-pass tool uses the same tool, but takes several passes to get to the final depth. Suppose you made a "Step" multi-pass tool that used tool 101 with 3 steps. If you applied that tool to a ¾” deep route, the machine would make one pass with tool 101 at ¼” deep, another pass with tool 101 at ½” deep, and a final pass with tool 101 at ¾” deep. If information is added in this tab, it can be entered in Imperial number format because it is converted to Metric when the program adds the macro to the spreadsheet. Otherwise, if entered in the “Spreadsheet” tab, it must be entered in Metric format because no conversion is possible from the “Spreadsheet” tab. If the 900 Tool is created or modified using the “Tools” tab of the Toolbox Options, you can use the provided interface. If created or modified from the “Spreadsheet” tab, go to the "Tools" sheet and on a blank row at the bottom of the listed tools, copy the previous line (make sure the tool diameter is valid). Next, modify the tool name to read "Router 901", or something that similarly matches the tool number. Now, modify the "Number" column to read 901, 902, or a number beginning with 900. When the program sees that number, it will then look to the "Multiple Tool Macro" column for the "Tool | Depth | Offset" information in the spreadsheet tab. Similar tool information must be contained on the "Default Tool Depths" sheet for that 900 Tool information to show up in the "Routing" section of the Toolbox. Copy a line down and edit the depth to read “900”, or something that will let the user know that the depth listed at that location is not valid. The depth is specified in the "Multiple Tool Macro" column of the "Tools" sheet, not on the "Default Tool Depths" sheet. This “Default Tool Depth” may be set to zero if desired. Tool Information Per Material Type Tooling information can be controlled from either the library items or from the specific material type. It is possible to control “Tool Numbers” and “Feed Speeds” all separately from what is defined in the library for that specific part, per material type. To control tooling information in the material type, simply open the material file and select the material to edit from the “Material Inventory” window. In the "Code" option you must enter in the follow statement: T101 F3|T102 F3. This statement is saying use Tool Number 101 (T101), for the route tool number override with a Feed Speed of 3 (F3) for the route override. Then it is separated by a "|" (pipe symbol). The pipe symbol is used to separate the "Route Tool Override” from the "Nest Tool Override". Then the statement continues; use Tool Number 102 (T102) for the nest tool override with a Feed Speed of 3 for the nest tool override. You would want to change the tool numbers and feed speeds to the ones you want to use for this material. Note: The “Nest Tool” override is needed only if a “Nest Tool” other than what was defined as the default in the tool file is desired for routing the nest borders. Otherwise, only the “Route Tool” override and its “Feed Speed” information will be needed. Vertical Drill "Pecking" Vertical drills have a pecking feature that allows you to drill into material with multiple drops. In the parameters, enter a pecking number for each vertical drill. G-code will then be written, causing the drills to make multiple drops (pecks) at increasing depths until the desired drilling depth is obtained. |
|||||
|
|
