|
|
What’s
New in Mastercam Router Version 9
|
Welcome
All Version 9 Mastercam Mill features are also included in Router Version 9. Click here for more information.
Listed below are the Router Version 9 product enhancements.
· Create, Next menu, Addins, Txtchain
· Right Angle/Compund Angle Aggregates
· Toolpaths, Next menu, Block drill
This new utility creates geometry for stair stringers. The bitmap on the dialog box is dynamic so you can see the changes as you edit the values on the dialog box. Using a Contour toolpath with the proper size cutter on closed stringer geometry will properly remove all material, leaving no islands, as long as the wedge angle is not too steep. If material is left using a Contour toolpath, try using an Open pocket toolpath with constant overlap spiral for the roughing style. With either toolpath, set the cutter compensation to Right and chain the part clockwise to avoid tearout on the corners.
If you make an open stringer, use a Contour toolpath with a straight cutter on the geometry representing the risers and the treads. Next, use a V-groove cutter (most likely a 47-degree cutter with a very small minor diameter) to machine just the lines representing the risers. Choose Single in the Chaining menu and start chaining from the outside going in towards the inside corner.
Refer to Mcam9\Router\Mc9\stair solid.mc9 to see how a typical set of stairs is constructed. All the components are on different levels, so you can turn levels off to get a better view of the construction. Remember, the stair utility only creates the geometry for the stringers and no toolpaths.
The following picture shows the settings for Mcam9\Router\Mc9\stair sample.mc9.
· The Stair run field sets the distance measured from the front of one riser to the front of the next riser.
· The Stair rise is measured from the top of one tread to the top of the next tread. This field is for display only. The individual stair rise is determined by the Finish to finish floor height divided by the number of stairs. Adjust the individual stair rise by changing the number of stairs until you get the stair rise you want.
· The Total run is measured from the front of the bottom riser to the front of the top riser. The geometry for the whole top tread is drawn and can be trimmed in the field.
· The Riser thickness is set to 0.005 inches larger than the material being used. This allows room for the board to fit in and also allows a bit of room for the 0.75-inch tool to pass through. A 0.75-inch tool will not fit through a 0.75-inch opening.
· The Top riser offset and Bottom riser offset create vertical lines for trimming the top and bottom of the stringer. If zero is entered as the top offset, the sides of the stringer will be connected with a perpendicular line. If zero is entered as the bottom offset, the stringer will come to a point.
This utility has been enhanced to allow different attribute settings for the inner and outer geometry, such as level and color. This change will make window chaining easier because you can either turn off one of the levels or use the color masking option.
The Multiple copies dialog box has been changed so you can enter the distance between doors instead of entering a spacing value, which previously included the door width. The ability to read in MicrosoftÒ Excel files has also been added. Microsoft Excel has to be present on your system for this to work. Door demo.xls has been installed in the Mcam9\Data directory. Be sure to navigate to this file on your system even if it looks like the proper path is displayed. The first column in the spreadsheet is for the width, the second column for height, and the third column for quantity.
This C-Hook has been added to allow you to place text along a curve or a chain of entities. You need a 2D curve on the screen before starting the C-Hook. In the following picture, the distance between the “e” and “r” was changed in the Advanced dialog box. You can return to the Text chain dialog box by pressing [Esc] or by choosing Backup before selecting Done.
The tool information on the Tool Parameters tab is no longer disabled as it was in Router Version 8. And Toolpaths, Contour, Depth cuts, Tapered walls is no longer disabled as it was in Router Version 8.
The Tool Parameters tab has a new right-click menu that allows you to easily save the current operation's parameters without choosing Main Menu, NC utils, Def. ops. This is available in all Mastercam toolpaths.
This addition to filleting creates a bubble in the geometry at the intersection of two lines. It only works with lines, not arcs or splines. This feature is mostly used in the upholstered furniture industry and allows the overcutting of inside corners so the outside, sharp corners of the intersecting male piece will fit in properly. A slightly larger radius than the radius of the tool is usually used to create the bubble. Chaining works the same way as it does in normal filleting. The direction of the chain is important unless you have the All option selected. Mcam9\Router\Mc9\clearance fillet.mc9 is a typical furniture part with the clearance fillets already created.
The Roll cutter around corners option has been added. Router Version 8 did not have the option, so it was hard-coded to always happen.
Roughing a flat floor can now be done with a straight cutter in Engraving. There is no need to use a Pocket toolpath. There is an additional option on the Engraving parameters tab to enter an angle for calculating an offset if a straight cutter is selected. This will keep the straight tool away from the geometry by exactly the distance that the tip of the V-groove cutter will end up away from the geometry. Use the XY stock to leave if you want extra stock left for the V-groove cutter to remove on the finish pass. Be sure not to leave more than the minor diameter of the V-groove cutter. The Remachining option may be the next toolpath you need to use if the straight cutter you selected was too big to fully clean out the corners.
Rotary axis for axis substitution (Rotary Axis button on the Tool parameters tab) is now available, as well as the ability to wrap engraving toolpaths (on the Engraving parameters tab) on shapes defined by two curves or multiple surfaces.
To get familiar with how these functions work, look at Mcam9\Router\Mc9\wrap on 2 curves.mc9 and wrap on surfaces.mc9. You can also use Chapter 7 in the Mastercam Version 9 Engraving Tutorial to try an example of this function.
This C-Hook maps NCI coordinates properly when using right angle/compound angle aggregates. Previously, all the work had to be done in the post processor and the aggregate block was not user-definable. Now you can define the aggregate block yourself and the toolpath will backplot showing accurate tool motion. This C-Hook converts existing operations that are created in Mastercam the way they previously were created. Define the plane to be worked in and machine the geometry. Then run the operation through the Aggregate C-Hook.
To access the C-Hook, press [Alt + C] and select aggregate.dll. The following dialog box should appear. The Operations list has a copy of all the operations currently in the Operations Manager. The section below that one shows aggregate blocks that have already been defined.
Select the Add Aggregate button to define an aggregate block and enter the parameters shown on the following picture. The aggregate block will only need to be defined once. After defining the aggregate block, you can just select an operation, select the block or station, and choose Apply.
Choose OK and the following dialog will appear to define the tool station.
There can be more than one station on an aggregate block, but you are defining one station at a time. The Tool Manager button will bring you to a list of tools in your current tool library. You can also select a tool by right-clicking and selecting Get tool from library. While in that dialog, you are able to change the library you would like to select a tool from.
The Tool XY angle sets where the tool is normally positioned relative to 0 degrees (3 o’clock). The software can then figure out how much to rotate the aggregate block to get the tool to the machining plane if it is a rotary block or if it can’t machine on the specified plane with that particular block/station because it is fixed. Clicking in the different edit fields can change the bitmap that is displayed and should help you understand what you are defining.
On some machines, you need to add the tool length (the distance the tool is sticking out of the collet) to the tool axis length (the distance from the pivot point to the bottom of the collet) and enter that number directly into the control. On other machines, just enter the tool length and the tool axis length comes from this C-Hook. It is a personal machining preference or a machine requirement.
The Display Diameter field is used for backplotting purposes only. The Aggregate Position to Reference Point Offset fields may or may not need to be filled in, depending on whether the aggregate block is actually offset or not. Each aggregate block and machine will be configured differently and you will need to speak to the manufacturer or reference the machine tool manuals.
Choose OK and you return to the main C-Hook dialog box that now displays the aggregate block and station that you just defined. Make sure the aggregate block you just defined is highlighted. The aggregate block can be selected for an operation if it has only one station. If an aggregate block has more than one station, the C-Hook would not know which station to apply, so you would have to select just the station.
Choose Apply and the Result List updates with the new toolpath. The original toolpath has become ghost-posted so you will not be able to run the post processor on the original toolpath unless you remove that in the Operations Manager. If you choose OK instead of Apply, you will exit the C-Hook. By choosing Apply, you remain in the C-Hook to map other toolpaths. More than one operation can be mapped at a time as long as the aggregate block is capable of machining all the selected operations. You can now go into the Operations Manager and backplot the new toolpath.
If you select Aggregate Selection Warning, the software will check to see if the selected aggregate block/station can actually perform the operation, such as trying to machine on a side plane with a tool that is fixed in the front plane. If you are using a fixed aggregate block and a rotary table, this option should be unselected because the C-Hook doesn’t know that the machine is actually capable of performing this operation.
If you select Translate Output to Machine View, the system maps the NCI coordinates to the machine view. If unselected, the mapping will have to be performed in the post processor. This function was enabled for all the post processors that are already written this way but still want to take advantage of the C-Hook.
Double-clicking on the aggregate block or the station brings you back into the definition dialog boxes to edit the aggregate block or station. Right-clicking in the white area that the aggregates are displayed in will bring up choices to save or get an aggregate to/from an HD9 file.
This toolpath is used for drilling rows of holes that are generally spaced in 32mm increments, like most panels seen in the panel processing industry. The drill block is user-defined though, so the spacing can be any distance as long as the holes to be drilled have the same increments of spacing and diameter as the drill block. The blocks can be defined as a vertical or horizontal row or a combination of both. L and T configurations are common. Some vertical or horizontal blocks have C-axis capabilities so they can drill rows of holes in either direction by rotating 90 degrees. Others are fixed in an axis. To define a block, start with one of the sample HD9 files and edit it. As soon as you read in the HD9 file that you want to start with, save it using a new name so you won’t overwrite the sample HD9 file.
Choose Main Menu, Toolpaths, Next menu, Block Drill to access the function. This toolpath does not work with points. It needs complete circles so the proper diameter drills can be matched up with the holes.
To change the spacing of the drills in a drill block, highlight a drill in the Tool Group area and change the X, Y, Z values in the Tool Position section. To edit the size of the drill, right-click on it and select Edit. You can also copy and paste to add another drill or delete a drill by using the right-click menu. You can right-click and rename the drill block or the drill itself. This will only append what is already in that field.
To try out this function, open Mcam9\Router\Mc9\ Drill Block Demo Metric.mc9. It is a cabinet part from KCDw. You can backplot the toolpath that already exists. You can also use Chapter 6 in the Mastercam Version 9 Router Tutorial to try an example of this function.
You can now read in DWG files to define sheets or parts.
Toolpaths can now be nested by choosing the Toolpaths radio button on the Parts tab. The operations to be nested need to be in the current Operations Manager so it might be necessary to import the operations into your current Operations Manager. Refer to Mastercam Help on how to export and import operations. It’s imperative that the geometry be saved with the operation when using this function for Nesting.
Multiple operations can be selected at the same time. When the toolpaths need to maintain their orientation to each other, such as when a single part has more than one operation in it, the operations need to be selected as operation clusters.
The associated geometry (geometry that is used to help create a toolpath) can be nested along with the toolpath if the Create new operations and geometry check box is selected (just like Toolpaths, Transform). This check box is located on the Work Offsets dialog box that displays when you select the Advanced button on the Parameters tab. This option will create a separate operation for each part that is on the sheet.
You can attach chains of non-associated geometry to operations that are being nested by right-clicking in the white area of the Parts tab. This option is only available after the operation has already been added. Highlight the operation that you want to attach the chains to and right click, selecting the Attach geometry chains option. This will bring you out onto the screen to select the chains to be attached. This option can be used when creating one operation or separate operations.
You will notice a legend at the top of the part display. A Profile is normally the outside of the part or the profile created from the tool center or tool edge. A Hole would be a chain that is inside another chain, designating the area inside the hole to be nestable area. Ignore would be geometry or a chain that is being brought along with the other chains but is not used in any nesting calculations. If a part is read in and the chains don’t have the proper designation, you can right-click on the part and select Classify chains as profile or hole. This will bring you to the graphics window and you will need to select a menu choice and then select the chain to change to that choice. The display background matches whatever your screen color is.
It is suggested to use the Only drill operations radio button when selecting operations that include drilling. Otherwise, each hole has a profile drawn around it instead of a single profile being drawn around all the holes, which helps speed up the nesting process.
You have the option to create a separate operation for each nested operation (select the Create new operations and geometry check box on the Work Offsets dialog box) or one operation per sheet (select the Each sheet has it’s own operation check box on the Sheets tab) or just one operation for all parts nested on all sheets (neither check box selected).
There is a Sorting button on the Parameters tab that allows you to sort the toolpaths using 4 different methods.
· Database order will machine the parts in the order that they were laid out on the sheet by the nesting algorithm.
· Next closest will go to the next closest start point from where the system finished machining the last part.
· Maximum vacuum will do all drilling operations first and then cut the smaller parts next, working from inside to out.
· Minimum tool changes will group operations together that are using the same tool, regardless of the size of each part.
· Group by sheet should be selected if multiple sheets are created and only one sheet at a time is going to be machined. This will be the most common scenario but some machines will have more than one sheet on the table at a time.
· Manually select order is only available after the nest has been generated. When you choose this button, the red shaded image is the first part that is going to be cut. The shaded images should be picked in the order they need to be cut. If you stop selecting the shaded areas before they have all been selected, the remaining parts will be added to the order of parts that were previously picked.
· Delete will allow you to delete specific instances of the toolpath by selecting the shaded areas one at a time.
The sheet can also be broken into user-definable regions. The previously mentioned sorting methods will apply to the region instead of the whole sheet if Sort by region is selected. All the sorting direction buttons located in the region definition area apply to the order/direction in which each region is going to be machined, not the parts in that region.
Common Nesting Parameters
There is an Only unused levels check box that is dependent on and under the Cycle levels starting with check box on the Parameters tab. This way, nested geometry doesn’t get mixed up with existing geometry and level names don’t get overwritten.
The Automatic sheet origins check box on the Sheets tab works a little differently than it did in Router Version 8. It previously only had an effect on sheets of one size. Now it refers to all sheets. If this check box is left unselected, all sheets and nested geometry will be placed on top of each other unless a separate origin is defined. More than one level should be used in this case so each sheet can be made visible by turning levels on or off. If all the sheets are placed out on the screen in different XY locations, then work offsets will have to be used for proper NCI output when applying toolpaths.
The Sheet margin on the Parameters tab can now be entered as a negative number. This allows the part to get a little closer to the edge of the sheet because the Part to Part distance and the Sheet margin are added together. The negative number can only be up to half as big as the Part to Part distance.
Two tool filter PRM files are installed (toolfilt.prm and toolfilm.prm). When you choose a tool from the tool library, these filters make it so only the desired tools are shown, like not showing drills and reamers when doing a Contour toolpath. If you want all the tools listed for every toolpath type, the easiest way is to delete these files. New PRM files will be automatically created as you make new toolpaths, just as the ones that are installed will be overwritten each time you make a new toolpath. The tools that are listed each time you do a toolpath reflect the way the filter was set the last time that type of toolpath was made.
The Contour, Ramp toolpath has changed. There is now a check box to disable the extra pass that is normally made at the final depth. This option is only available when the Depth radio button is selected. It has been added for woodworking customers that cut laminated material and want to vary the depth of the tool as it’s progressing along the cut so more of the tool cutting edge gets used. When cutting laminated material, the tool wears quicker in the spot of the lamination so varying the tool depth along the cut will increase tool life. To take advantage of this feature, set your Feed plane above the part as you normally would. Set your Top of stock at the bottom of the part and the depth should be how much more you are willing to cut into the spoilboard or how much more of the tool cutting edge you want to take advantage of (if your part is on a pod). Set the Ramp depth to the difference between the bottom of the part and the final depth. Deselect the Make pass at final depth check box. Open Mcam9\Router\Mc9\Ramp contour.mc9 and backplot or verify the toolpath in the front view to see the ramping motion.
All Version 9 Router toolpaths (except Engraving) support Multiple heads (main and piggyback). Open Mcam9\Router\Mc9\Multi head.mc9. When you enter the Multiple head dialog, the main head is always available. Right-click and create the number of piggyback heads that you have on your machine and then highlight each head individually and enter the XYZ offsets. The display at the right will show the heads but they will not appear when backplotting or verifying the toolpath. After the heads have been created or retrieved, you need to select the check box next to the heads that you want to drop. The appropriate code will be output in the NCI file. Your post processor must be written to read this information correctly. The Multiple head configuration can be saved as an HD9 file along with a drill block of the same name or saved by itself with a different name.
There is an Art Library that is optionally installed in your Mcam9\Router directory that consists of thousands of clip art files. You can also leave the files on the CD and navigate to them from the converter. These are stored in an MZ9 file format, which is a compressed MC9 file. To read these files, press [Alt + C] on your keyboard and select MZ9.DLL. The menu on the left will display the options to read or write an MZ9 file, as well as read or write an entire directory. When reading in an individual file, there is a viewer available to browse the files. There are also PDF (Adobe Acrobat) catalogs that are installed, if you would like to view the available clip art using that method. This utility can be a useful tool for compressing any MC9 file.
Updating Posts From Previous Versions
Since Version 9 is a major release, posts that have been written for any earlier version must be updated to ensure proper functionality and safety. In addition to the changes the update utility makes to a Version 8 Router post, most Version 9 Router posts will need additional edits to work with Version 9. Please contact your Mastercam Reseller for more information. This function is found under the NC utils, Post processor menu.
For information on what this update procedure does to the post processor, see the UPDATEPST9.HLP help file in the Chooks directory.
The following changes are made if you runt the Update utility.
Questions 159, 1503, 1520,
1521, and 1530 are added to all post processors.
159. Show first and last
position as fully compensated in simulation? n
1503. Write transform
operations (0=transform ops, 1=source ops, 2=both)? 1
1520. Display a warning when
cutter compensation in control simulation finds an error? n
1521. Number of controller
look-ahead blocks for CDC in control? 2
(Note: The 1521 question is for future use.)
1530. Ignore work offset
numbers when processing subprograms? Y
The 1530 question directs Mastercam to ignore the work offset numbers when processing transform operations for subprograms. If the response to this question is Y (yes), transform toolpaths will create a single subprogram number even if the work offset numbers do not match in copied patterns. This happens frequently with rotate transform toolpaths. Ignoring the work offset number prevents identical subprograms from being generated.
Router posts have this
additional new question:
5001. Name of HD9 definition
file?
Post Numbered Questions Information
The new names for these files are Mill9.PNQ, Lathe9.PNQ, Wire9.PNQ and Router9.PNQ. PNQ = Post Numbered Questions. These files provide additional information about the numbered questions in the post processor.
Support for Full 360 Degree Arcs
With some simple changes to the post, it is now possible to output full circles as a single 360-degree arc move instead of two 180-degree moves. Refer to the Post update documentation mentioned below for details.
Additional Post Changes
All new post information specific to Version 9 is documented in a file called Post Processors - What's New in V9.PDF. This file is installed in the same directory as the What's New files for each product (C:\Mcam9\Whats New).
MCU Light v2.1 (a substantial sub-set of the MetaCut Utilities) is included at no charge with Version 9.1. The MCU Light OEM version for Mastercam requires a Mastercam security device (SIM). MCU Light is not included with Design.
MCU is a powerful set of utilities for your toolpaths that will quickly become an essential tool throughout your shop. MCU integrates directly with Mastercam, and also works as a stand-alone application, that helps you problem-solve and analyze your toolpaths both before and after post processing.
Free Trials of Current and Future MCU Features
As an MCU Light user, you will automatically receive a free 30-day trial of the full MCU v2.1 software. The full version of MCU includes G-code verification, graphical editing and comparison, multiaxis backplot of NCI files, and much more. As new features are released for MCU, you can try them for free just by downloading and requesting a trial version. Talk to your Mastercam Reseller or check the MetaCut Web site for newly released MCU features and versions.