CNC Coding Guide

Back to home

Complete guide to use CAD/CAM, CAD and CAM in Lathe on NX

This is a complete course from the beginning to the making of your first model and finally a manufacturing

You going to accomplish both sketch, model and manufacturing

To be able to follow this instruction you supposed to get a verbal walkthrough, this because of some minor grips are not shown or explained. Every important step is in the instruction, so you can make your way thru anyway

  • 12 dec -18. I'v started the process to correct the written language, bits and pieces of it are ugly thanks to auto translate

    This video are made the same as the instructions, some may differ, I made the video back in 2013, click here

    Create a file

    Click New in the file menu

    Select "Model" with millimeters or inch as the unit.

    Note The NX's difficulty in managing file and directory name. NX does not accept spacing, letters and numbers mixed, nor are special characters such as ÅÄÖ% and more that are completely prohibited. Unfortunately, the problem usually does not show up before the end of your work, at the end, and makes all work can be in vain. Use Under_score to divide numbers and letters and also as spaces, newer versions cope with this on a more mature way, V6-7.5 not at all

    Choosing the right Plane that fits the manufacturing

    To get the manufacturing to work properly, it requires that we have drawn solids in the right plane. If we miss the right plane now, the machining will not work well or even at all.

    The plane we draw on has confused enough X as the "center" on the round detail, it should of course be Z if we are turning. NX will change the X to Z when we set up the manufacturing later, and it takes no account of the fact that we incorrectly plotted around the z axis, then the z axis changes to an unusable Y-center axle.

    This one needs carefully considered. If we do this right now, it is a good to way to not find a machining that doesn't work later.

    Click Sketch and move the pointer over the drawing field without clicking. A default plane pops up if you use the option Infered as method, this is the plane we want to use in both lathe and mill, click OK

    Text on picture = hold the pointe above the drawing center, but do not click

    Draw a sketch that fits a lathe solid

    We draw in X-minus. Y representing the Diameter is indicated in the Radii measurement as we will "Revolve" the contour to a cylindrical detail. You can enter the values as a formula if you don’t want to count, put the dia 50/2 (dia divided into 2)

    You can choose between X and Y coordinate and to use line length and angle.

    XY-mode does always refer to CSYS (your start point in the drawing)

    To end the figure by tying up all lines, use the Help functions that appear.

    The figure can’t have any openings

    Text on picture= draw a profile with radii measurement

    Tie the lines together using the help lines that pop up if you drag the pointer past the origin/start point (CSYS)

    Create a cylindrical solid

    Finish the sketch. Send the small arrow next to the Extrude to find the Revolve command.

    Select the entire shape in select Curve.

    Select only the center line of the Specify Vector.

    Now Revolve everything automatically

    Finish by clicking OK

    Text on Picture

    1 Chose whole figure

    2 Chose the centerline

    3 finish the sketch

    Threading on Model

    This video covers this section start here

    If you want a thread with the model, the problem arises that thread usually has a camfer in on the start. You can not thread this in the usual way, you need some extra steps.

    There is another more clever solotion on this, I’ll add this later.

    Start by creating a new plane at the end of the thread

    Click this on the end

    Then create thread with thread command

    Select the cylindrical surface

    When you choose, a ghost field pops up without any information whatsoever.

    The sentence is so that we choose the plane, click on the square.

    Now, however, an unidentified function is added, we need to enter direction, click OK for guessed thread direction. It says that "tool body complete out..) Is the wrong direction selected, remove the thread, rerun the command, but then select Reverse Thread Axis.

    The selection of the thread setting is done as follows, for example M40x2 (x2 indicates Pitch)

    Major diameter is the diameter you have created in the model.

    Minor Diameter is above minus Pitch

    Length is the length of the thread from the starting plane

    Pitch is ascent

    angle is the thread angle, which on all modern threads is 60 degrees

    Create a blank

    What is called blank in NX is the form of the material before machining

    The blank is created by making a Extrude of the outer circle at the largest diameter in the rear of the detail, just click on the corner, do not light the whole plane.

    It is possible to catch the Extrude and pull it as big as you want the blank, look at the center line after the pull position.

    Important! Boolean must be set to None, so that detail and blank should not be joned togheter

    If you want greater diameter than the drawn solid, you have to plot that diameter as a circle in the plane

    Text on picture = Make a Blank (material of the workpiece before manufacturing)

    Make blank Transparent

    After Extrude wins the fine solid we made.

    To bring it back, we go to the top menu Edit, snooping around the "edit object Display"

    First, we choose everything, just highlighting so that everything gets highlighted.

    In the next mode, there is a slider that we set at about 50%

    Now is shiny semi-transparent


    Create a manufacturing

    Solid ready, click File, New. Select the Manufacturing tab.

    Set your units to Inch millimeters, also select turning (Express)

    Text on picture:

    Manufacturing name

    The model name

    Define details for processing

    In order for manufacturing to know which is solid and which is blank, we must communicate this to the NX.

    Click + on the MCS_SPINDEL

    Double-click WORKPICE

    Select Part with Specify part, wait with the pointer for about 3 seconds until 3 … (dots) pops up under the pointer, then click. A multiple choice window pops up, you can choose inner or outer by hovering the pointer over the options. Select the inner.

    The same goes for Blank, but then we choose the exterior.

    Specify Check doesn't help us in this situation, so don’t use that

    Text on picture: Choose between inner and outer, choose inner

    Text on picture: Choose outer

    Processing area

    NX will now itself determine the machinable area between blank and solid-

    Click + to open up turning WORKPICE and click once on this one (double click in NX11).

    It looks like the picture is all good, the Z-axis is called Z-axis

    Did your detail got wings or ghost fields in other places, remove everything you struggled with and start over, you haven't done the right thing when it comes to choosing the plane at first.

    Text on picture

    1 single click

    2 processing demarcation ( blame google translate for this)

    Create operations

    Since there are already two predefined tools in turning, we can go directly on the create operation.

    Click Create operation. Unlike milling, the Type field for turning has no other options

    Operation subtype displays different manufacturing variants, hover over the options to display text.

    We choose Rough_Turn_OD (rough turning outside)

    In the Location field we got 4 important choices.

    Program: Default 1234, nothing we need to change

    Tool: There are two tools, select the 80 degree C-insert

    Geometry: We're talking about the processing, we were set up blank and part, and it should be turning_workpiece.

    Method: Rough, Finish, Groove, etc., select the correct

    Name can be changed to what you think fits, but note the format of the name

    Create the operation Rough_turn__od

    Rough Turn OD-operations Panel contains lots of options we should not care about at present.

    We can note that the machining area has become beautiful pink.

    The pink field is that which NX decided that there are materials to process and that we process with this OD operation.

    We do not need to make any adjustment at this time, the machining area is good enough to test as it is.

    We must generate this approach to see where the machining will end up.

    Scroll down and look for the button for this:

    Text on picture: generate tool path

    This icon needs a click as soon as we change something in the processing, the function generates the actual tool path. It also tells us if something is wrong or if some surfaces or holes are not made

    You now have a chance to study how the tool moves in the material, red stretch usually mean fast feed, light blue for processing with G01, blue/red both feed and fast feed, usually in holes. However, the Verify function provides a clearer picture of the processing

    Cut Regions

    Since we have to steer the machining that in this case it does not run on the plane we have to put a radial plane that tells the NX that we do not want to process behind this limit.

    Select Radial Trim plane 1, Limit Options > Point, click on the top of the smallest delimiting diameter.

    Do not forget to regenerate after this

    Text on picture: click on the top of the lowest diameter

    The Cut regions apply only to the current operation and must be redone when finishing.

    But, there is a built-in weirdness, normally you start of course with that flat bit, on facing, choose a Axial plane, this remains even in subsequent operations and prevents all futured turning, wierd, in know, but as a solution we run the facing last.


    The Verify function displays the processing graphically and the button for this is in the same field that generate is located.

    Choose 3d and run through the operation, this run also creates your IPW if you need such a

    If you want to run the entire program go to Operation Navigator, select WORKPICE, right click, go to Tool path, and select Verify

    Post process

    The program is basically complete, it only needs to be adapted to the machine and the programming language that the machine is using, the process is called the post process and is located on the icon bar and in the right click.

    Select WORKPICE, right-click, select Record process.

    Choose a suitable Lathe, ToolTip Lathe think we work well and are standard in the program. you may add your own or downloaded post processors that you can load by clicking Browse.

    The Output file box is totally allergic to the ugly name, you have the ugly name of your directory, file or similar you can forget that the posting should work.(it seems to work fine anyway in NX11)

    But since we have been talented and learned this, everything will go well.

    Select mm or inch in Settings when these original posts are made in the United States and have inch as standard

    You will be warned that the post measurement may be changed and your selected measurement are not correct, we already know this, so click OK this.

    Save a manufacturing

    When you are ready and want to shut down, everything will be saved.

    You have 3 files open of which 2 piece are yours, one file belongs to NX

    If you take Save all you will receive an alarm that the file turning_express. PRT cannot be saved. This file we do not want and can not save so cancel the error message, your two files are saved in a good way

    Threading operation

    This video covers this section start here

    If we have drawn a thread in solid, it is easy to process the thread

    Create a threading OD tool

    Create a THREAD_OD

    We get some mysterious options, including demanded Crest, which means back crest or in this case the top of the thread. We must select this in a specific order that automatically gives thread start and end.

    When Crest Line is selected it is the highest point on the thread, then we can select Depth and Angle in the Depth Option box and enter the measure of the thread, pitch and 180 degrees. Do not select End Line

    We also open the Offset field to be able to specify the length of the thread. Now we chose this whole length, but we should only thread a shorter part, minus the End Offset makes the thread part shorter.

    CNC Coding Guide





    Google Play Store
    My Youtube channel