This is a complete course from the beginning to the making of your first sketch, model and finally a nice manufacturing with a ready-to-use CNC program You going to accomplish both sketch, model and manufacturing
-12 dec -18. I'v started the process to correct the written language, bits and pieces of it are ugly thanks to auto translate
If you feel to pay any amount of money to me for the work with this use this link paypal link
We start all with creating a model
Go to File > New or use the icon with the same name.
choose the Model tab, make sure Millimeter or Inch is selected for your desire
NX does not handle file names, directory names, and more very well. It is important to "format" the name correctly. Do not use Åäö and%-like characters.
Spaces shall be represented by _ (underscore), the same applies if you mix numbers and letters.
The default directory does not work good at all, creating a directory called CADCAM on your C drive (c:/CADCAM) is the best choice
Text on pic = No funny names
A solid is an "air tight" form, we create the base of this form in 2-dimensional mode to create the air tight volume on this later
To get the X, Y and Z coordinates right from the start you have to follow a special pattern when drawing in Sketch mode. Missed this now, it will give you problems towards the end. Take note of the X,Y and Z-directions, really a p.i.t.a. to change later
Click the Sketch icon at the bottom (arrow) Make sure that Inferred option is active in plane method, Drag the pointer over the drawing area so the square lights up around the arrows, don't click! Select OK
Text on pic = Hold the pointer over the sketch area, but do not click
All the details we will make are based on squares and circles.
Turn up the CSYS (as that 3 pointed Arrow shape is called) so that you have Y up and X to the right, Z should point you straight to your nose
Choose to draw a square
Make sure to be in the position with a square of 2 digits in the top left, dimensions are entered and you have the option WIDHT Height or X and y, x and Y options keep track of whether you are on the minus or the plus side of the figure. In W and H mode, you must be in the correct quadrant with the pointer. See figure below
Type 0.0 to set zero, then type the dimensions for the size of the square, right-click and choose OK
After as we previously clarified that everything is circles and squares is a negative radius only part of a circle, select the Circle function and click on the inner square corners. Make hole Ø to Ø20 (RADIUS 10). Click on the other three corners without exiting the command
We need to trim down the circle and a small part of the square so that it becomes a negative radius.
Select Quick Trim. Click the lines you want to remove.
Center-Marking or point for hole-extrusion needed.In many cases a mark in the centre of the holes with a + (point) in order to be able to select them when creating holes later. In this case, it is not necessary for the centre points to be created by previous drawing parts
Select Finish Sketch to enter 3d mode
Select the Finish Sketch to get over in the position where we can create a solid of our stretch.
The first extrusion is the outer square. Select Extrude and double on one of the outer lines, notice that connected curves must be selected. If the O-selected is selected all the Infered is used.
Extrude in Minus so that you as long as you can keep the drawn lines on the model top.
You can also pull out the extrusion if you pull the purple arrow
Extrude up the top as you extruded down the bottom part
The holes are extruded with command Hole. Point in the box is the point to represent the hole center.
Enter diameter 10
Depth limit can be through Body, thus consistently or as in the box below, as Value. It does not make the hole too long, as the hole that does not contain anything is outside the piece
Select File > New from the top menu. Select the Maufacturing tab and select General Setup. Make sure the units are in millimeters or inch
The name of the manufacturing will be your Modelnamn + _ setup_1. Prt, folder shall be in accordance with the naming conventions of NX. Part To reference is your model.
You should be in the operations Navigator mode and in Geometry View
We need to tell the NX which your model you want to use and create a Blank, which will represent your workpiece before milling before processing.
Start by selecting Specify Part
Blank Geometry Choose as Auto Block, then the size represents the model's extreme values. You can enlarge the Blank so that it provides processing on top and sides, but in this case, we allow all values to be zero
In this General Setup there are no default tools. So we must create them from new.
Click Create Tool
Type should be mill_contour, Tool subtype containing different tool options, select Mill which is a regular endmill
In Location Select tool switches the location
Call the tool for something you recognize, but remember how things get called according to NX.
Since I deliberately made a mistake in this operation, we get an error message. I do not reveal the error, it allows you to easily figure out yourself (NX 11 will handle spaces, 7.5 not at all)
We have to put a number of values on the tool, diameter is most important.
Length is the total length of the endmill, Flute Lenght is the length of the flutes, what is shown yellow on the tool
We use Mill_Contoure as the Type
Operations subtype contains lots of different processing options for processing, you can use for example Z_level_profiling if you want to drive around the outer edge of a detail.
We use Cavity_mill quite often when it clear a number of different machinations.
Program 1234 does not need to be changed
Tool, choose your suitable tool
Geometry: WORKPICE (and nothing else!)
Method adapts to how you intend to process, options Finish and Rough
Names can be changed to something you recognize, think of the NX and its naming rules.
Make sure the WORKPIECE is your Geometry
Click Specify Cut Area
Select the area you want to process. Sometimes you also have to choose the edges, but not now.
Go at the bottom of the box and generate your choice, NX calculates the tool path now
If you change something in the operation, you must regenerate
The generation creates the tool path, which includes quick runs and machinations, quick feed is red and blue, light blue is cuttin in the material. White and yellow represents approach and departure.
Verification shows how the tool processes in the blank
But it also creates the new model that will be after you have worked away, this used the nice run then to know where the material is already gone and you do not have to drive again. Then we have to choose to create a IPW (in process workpiece)
The operation is basically the same as rough driving except that Method MILL_FINISH.
In this operation the same as the rough run.
Select surface and generate. Don't forget to save on
(Not in NX 11)
Select Drilling, drill that you created and Method Drill_method, even here you can call the operation for any name.
We skip the next phase, which is the choice of diameter, we have gone through in the choice of Mill and it looks alike here
In drilling we have 3 choses.
Select holes can be done by selecting > All holes On Face and selecting Top surface. If you have more different large holes you can delimit the diameters before clicking the surface
Specify Top Surface selection is also Top surface, but it should be chosen as plane
The bottom surface choose either the plane and the bottom surface or the drill depth with ZC Constant, this does not require any click on surfaces
Generate the drilling and study the tool path. Check carefully that the drilling really goes down the hole, it does not do it, you have done something wrong in your model or tool choise.
Red path represents the coarse feed (G00) light blue corresponds to the working feed (G01), when the colors are mixed, it is both types, in this case G01 down the hole and G00 up out of the hole
Now all share ready, it's time to verify the entire run as a package.
Select Workpiece in Operation Navigator on the left, right-click, select Toolpath > Verify
Would! be replaced with a stop sign, right click on the Workpiece and select Generate in the menu, OK on all questions
Now everything should be adapted for a CNC machine.
Stand on the Workpiece, click the post Process, either on the icon menu or with right
Select Mill_3_Axis as the post processor (or the assigned to you)
In the File Name box you should have the names right, otherwise this does not work at all, you can not post if you have not followed the rules of name making.
Also choose millimeters in the units as when needed, in this post, the Americans have poked in both inchs and feet in NX, we don't want to use that if we are metric guys, our parts become 25.4 times smaller .
You get the code in the format we ordered, it is almost ready.
You need to change some things, including the tool change rows that have the introduction: 0030 and so on, this is necessary to do before we even try to bring anything to the machine.
The one with good memory knows that the sign:(serial file transfer between computer and machine, : is the program name) Indicates the program name that the machine will assume, so you have 5 tool changes, the machine divides your program into 6 parts, completely unusable in other words
Create a tap in the Create Tool as usual, Diameter, Pitch and save this.
Select Create operation, drilling and tapping operation
Select holes according to drilling on Cycle – Standard thread
-Select OK at Number of Sets
-click Depth, select Bottom Surface or Model Depth for continuous threading. You can also set the depth with the option Tool Tip Depth, then you get to enter the thread length
-OK, OK and generate
Thread milling works both with thread made in solid and with a straight hole, but unlike lathe threading, the cutter operation does not inherit the properties from solid thread.
-Create Operation – Mill Planar-Thread Milling
-Specify Hole or Boss button
Change From And Pitch to Specify, mark the mantle area in the hole
Form shall be Metric
Pitch is your ascent (which is the same here and on the tool)
-Threading drill Size same as thread inner diameter or drill diameter
-Depth must correspond to thread depth
-Major Diameter (thread YD)
-Minor diameter (drill Diameter again) (Dia-Pitch)
-Lenght Same as thread length
In order to be able to identify what the processing does after generation, among other things to find faults, all feed types have a pre-selected color, for example where tools cut into materials become the tools light blue, quick feed becomes another another color depending on departure or approach.
The table below shows the appropriate types.