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
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
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
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
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)
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
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
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)
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
Solid ready, click File, New. Select the Manufacturing tab.
Set your units to Inch millimeters, also select turning (Express)
Text on picture:
The model name
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
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
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)
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
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
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
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.
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
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.