Import your part

  1. Create a folder on the desktop: bracket_yourinitals (mine would be _psr)
  2. Copy the ‘read-only’Solid Edge se_bracket.par file into your new folder. From the MS windows Start →All Programs, open Unigraphics NX.
  3. From the top menu items: File → Open→Files of Type, scroll down to Solid Edge Part Files [*par]: navigate to your folder and double-click se_bracket.par Note how this changes the file extension to .prt, and makes it a UG file now. Save as bracket_initials.
  4. From the top menu items: Application →Modeling
  5. From the top menu items: Preferences →User Interface →Reset Window Position. (Note: the UG window is always left as the previous user had it. This step brings us back to ground zero. You will personalize your windowas we go along). Also, at this point please be sure the Save layout at exit box is not checked. If it is checked, un-check it. Hit OK
  6. The mouse center scroll wheel changes image size. From the top icon menu:
    fit the screen hit shaded and trimetric view buttons.
  7. We are going to machine this part, so need a material ‘blank’ to do it. From the left menu icon bar click on insert a block and give it the dimensions(5.5,1.625,4.25) when the Block dialog opens. Note also that the command line at the very bottom of the screen says: Select origin point – Specify inferred point. UG wants to know where to put the block. Move the cursor out over the edge of the outside lower circle as shown here, and the block corner will be placed on the purple diamondthat your screen shows, when you left click. Hit OK, and then fit the screen again.
  1. Looks confused here, doesn’t it? Don’t panic. From the top menu items: Edit →Object Display. When the class selection dialog appears click on the upper left corner of the blank you just inserted. The blank will turn the selected color (red). Hit OK. In the Edit Object Display windowclick on Color, change it to dark blue, then slide the Translucency slider to 50. This is a percentage. Hit Apply. Note the part is now seen partially inside the blank. Hit OK
  2. From the top menu items: Edit →Transform and click on upper left corner of the blank as before. Hit OK. In the Transformations dialog select: Translate →Delta and fill in (-0.5,-0.282,-0.5)hit OK and then hit the Move button then Cancel (or it will move again.)
    Grab the rotate button from the top menu and spin the model around.
    The part is now entirely inside the blank, and ready to machine.

Here we imported a part directly opening a Solid Edge part. If you bring in something from other software: AutoCAD or Cobalt (STEP or IGES), or from Solidworks (parasolid or STEP) the steps are the same except:

Open a new, empty UG file, and use File →Import, and follow the instructions to import the part, and pick it up from step 4.

Be sure to save your work frequently. Do not leave things locally on the lab computers.

Setting the Machine Coordinate System

  1. Application →Manufacturing. In the Machining Environment Dialog select mill_contour in the upper box, then again in the lower box, then hit Initialize.
  2. And, to be sure we are all looking at the same screen here:
    Preferences →User Interface →Reset Window Position.
  3. There are (annoying) flyout menus on the right side of the screen. Double click on the third from the top: Operation Navigator. The Operation Navigator window will open on the drawing screen. Tear it off if necessary, then resize it and push it to a corner, out of the way.
  4. On the top icon menu bar, at the far right, are the 4 Operation Navigator views.

    The default, and the one you see now, is the Program Order View. We will be using the Machine Tool and Geometry Views, 2nd and 3rd respectively, from left. Click on the Geometry View now. Note the Operation Navigator window you resized has changed to Geometry.
  5. The part file has been ‘seeded’ with a coordinate system: MCS_MILL Open the tree and you will see that the file has also been seeded with geometry: WORKPIECE.

    Note also that a new “machining” coordinate system XM, YM, and ZM has been created directed over the original coordinate system in the bracket. So we’re not confused here, turn off the WCS from the top menu bar: WCS →Display.
  6. Double click on the in the Operation Navigator. Notice that the MCS has changed to a dynamic mode. Click, hold, and drag the cube in the center of the MCS from the center of the bracket up to the nearest top corner of the blank:

  1. Next we must rotate the MCS about the + X axis to get the Z to be pointing up.
    Pick the Rotate origin as shown below.

    In the dialog box pick and hit Apply then Cancel and we have the system where we need it.
  1. To insure that we rapid traverse above the part we are going to set a Clearance Plane. In the same dialog box pick Clearance→Specify. Type in 0.1 in Offset (It is already highlighted). Then move the curser out over the top (XM,YM) plane and quickly pick the top plane. It will turn selection color (red) and show a direction arrow up.

    Hit OK and OK again. We have now put the machine coordinate system origin on the upper left corner of the block, as we did when we cut our initials in wood.

We are now ready to define the geometry. As we move from the gantry to the Benchman VMC later in the course you will see the different coordinate system requirements.

Defining the Geometry

  1. In the Operation Navigator window double click on the WORKPIECE icon. The MILL_GEOM window will open. Here is where we tell UG which is the part and which is the blank. The window defaults to the part icon.

    Pick Select and move the curser out over the part. Leave it until it turns into a
    + . . . symbol, then click. Pick the number 2 box. This allows the software to go ‘inside’ the blank and pick the part, which is now outlined in purple. If you got it right, when you click on 2 the bracket will turn the selection color (red). Then Click OK in the Part Geometry selection window.. To double check, pick Display. The part will outline in purple.
  2. Next, do the same for the blank, the center icon in the MILL_GEOM window. Click on Blank →Select. Then move out over the part in a place were only the translucent blue blank is under the cursor and click on it. If you got it right, only the blank will turn red. Click OK in the Blank Geometry window. To check pick Display and only the outline of the blank will be highlighted in yellow.

That’s it. You have defined the geometry.

Create a tool

  1. At the top of the left hand side icon bar are the Manufacturing Create Operations icons: The top is create operations, next is programs, then tools, geometry and method. We will be using only operations and tools. Tools first.
  2. When you click on the Tools icon, the Create Tool dialog opens. It defaults to Endmill and gives it the name MILL. Click OK
  3. The Milling Tool – 5 Parameters window opens, and the (D) Diameter entry box is highlighted. Type in 0.25 and hit OK.We have created quarter inch end mill tool call MILL

Create an Operation


  1. Click on the create Operation Icon, Top left button. The Create Operation window opens, with the top left operation Subtype default selected: Cavity Mill. We will use this one.
  2. Change the Use Geometry Menu. Pull down and select WORKPIECE as our geometry.
  3. It picked the only tool available, the MILL, so we can leave that
  4. Change the Use Method: pull down and select MILL_FINISH.
  5. Click OK.
  6. The CAVITY_MILL window opens, with the Stepover Percent cut method highlighted at 50% tool stepover. Leave that, as well as the 0.25” depth per cut (for now) variable and simply hit the generate button directly above the OK button The process will go faster if you click off pause after each pass button.
  1. The blue lines are cuts. The red are rapid moves (G00’s) the yellow are entry moves (note that the default is a spiral for pockets, an arc for side entries). F5 washes the screen.
  1. On the far left icon menu bar at the bottom are the Manufacturing Operations Tools. At the top is the generate icon. You can re-genereate tool paths at any time with this button. The third from bottom is the CLSF formats output. This basically ‘paints’ the screen for UG
  1. On the top icon menu bar pick the Geometry Operations Navigator button, then click on the WORKPIECE icon to highlight it.

  1. Click on the Output CSLF button from the left menu (shown above). Click OK in the dialog box that appears. The paint screen information output appears. Just close it.
  1. The next icon below CSLF shows a little machine . This is the postprocessor button. Click it and pick the gantry (the lathe is highlighted) and click OK. Then wait. The Gcode is being created. The information box opens showing the code. Admire all your hard work writing the 4,409 lines of code, then click the window closed. Your done.

Finishing Touches

  1. Also in the Manufacturing Operations bar is the verify icon: This will simulate the tool path. Be sure WORKPIECE is still highlighted in the navigator, and click the verify button. At the top of the Tool Path Visualization window pick Dynamic, then at the bottom click the right arrow ‘play’ button: . Admire your hard work some more. Then click OK. In the future you may want to make the image smaller so it will run faster, and rotate it for a better view. And, of course, if we decide to actually cut this part we have some pretty fancy fixturing to do.
  2. At the very bottom of that bar is the Shop Documentation button: Pick it and select Advanced Operation List (HTML) from the list. Click OK

  1. Minimize UG and navigate to your se_bracket folder. In the folder you will now see 7 files:

    the .par is the original imported Solid Edge file, the .prt is the UG file you are creating. The cls is the paint code. The .nc file is your text file containing all the Gcode, ready for the gantry. Double click on the .html file. If you put this file, along with the .gif files created for it, into your web site and link to it, your work will be displayed.
  1. At the top menu, click on the Frontpage editor:
  1. Customize your page. Add a link to the NC code file, and the part file that are both in the same folder along with the images. Note: if you change the file extension of the Gcode from .nc to .txt, the code will open directly from the web page. A nice touch. Now, when you put the folder in your Sites folder you will have access to all the work you have done today.

This is obviously a simple application. As we go through the semester will take on increasingly complex parts. But the steps will not change:

  • Import the geometry
  • Insert a blank
  • Create a coordinate system
  • Define the geometry
  • Create your tools
  • Create toolpaths
  • Generate Gcode, and verify the part
  • Create documentation

Notes

  • The middle button scroll button on the mouse can be used to change the size of the part in the view. Give it a try
  • UG is ‘Microsoft Compliant.’ Go to a blank area of the top and left side in both the modeling and manufacturing menu bars and right click. Turn on/off some of the menu items to see the effect on the screen.
  • I find it useful to ‘rip off’ some of the menu bars, particularly the manufacturing create and manufacturing operations bars. They just seem more accessible that way.
  • It is always good practice to create files in separate folders. This organizes all support files: NC, clsf, html, etc. that are created along the way. And it makes it much easier to organize your web page.