Adding 3D step model | Altium Designer tutorial

This tutorial shows how to add 3D PCB step model in Altium Designer.

For more PCB design tutorials visit- Altium Designer Tutorials

Suppose you have a component which has a schematic symbol and footprint but does not have a 3D model. As an example, consider the case where we have the Atmel's ATmega8-16AC which is a 8bit microcontroller. This microcontroller chip has a schematic symbol and footprint as shown-

 
Now if the schematic symbol is double clicked it brings up a new window showing the properties of the component. There under model you can see what other files are attached to it. Here it shows that footprint is available to it but not the 3D model.

Select the footprint and click edit. This will bring up the footprint information. This is shown below-

Now we have attach a 3D model to the footprint. To do so first we require the 3D model for this chip. To get the 3D model we can either make a new one or download an existing one from sites like 3Dcontentcentral.com.

Here we will download the 3D model of this chip from the 3Dcontentcentral.com and attach to the footprint.

To do so, follow the steps.

First go the 3Dcontentcentral.com and download the 3D model step file from the website. For this make a search and you will be shown the available model if the site has one. This is shown below-

Once the component is found, go to the download section, select the Format as STEP(*,step), and version as AP214 as shown in the figure above. Click the download button and download it to a suitable folder in your hard drive.

Now to attach this 3D model step file, we have to open the footprint of the ATmega8-16AC chip and attach the 3D step file there. To find the library that contains the ATmega8-16AC chip make a library search. Here in this case, the footprint and schematic symbol of the ATmega8-16AC chip was inside an integrated library called Atmel Microcontroller 8-Bit AVR. This is shown below-

To get the footprint only, open the integrated library and altium designer will ask whether to extract the integrated library. Select Extract the integrated library. It will be extracted in the same folder containing the integrated library, see above picture.

Once the integrated library is extracted, the schematic library and the PCB library(footprint library) will be visible in the project panel as shown below-

Now select the Atmel Microcontroller 8-Bit AVR.SchLib and then click on the SCH Library tab at the bottom of the project panel and select the ATmega8-16AC. This is shown below-

This is the schematic component/part to which the 3D model will be attached.

Now having noted footprint used for this schematic part, we continue to select its corresponding footprint. To do this go back to the project panel, select the Atmel Microcontroller 8-Bit AVR.PcbLib and click on the PCB Library tab at the bottom of the panel then select the 32A_M footprint from the library as shown-

Now go to 3D view by clicking on key 3 on the keyboard. This brings up the 3D view as shown-

In altium designer, sometimes 3D view will not show. This is because the 3D view is not enabled. In such case then while in the 3D mode, press key "L" and select "Yes" in the Show simple 3D bodies as shown below-

Now go to Place menu and select 3D body as shown-

This bring up a dialog box that allows us to attach the 3D step model (downloaded earlier). In the dialog that appears select the Generic STEP Model, and click on Embed Step Model. Browse to the location and select the step model file that you had downloaded earlier(or the one you want to attach). This process is shown below-

Once the step model is opened the 3D editor window will have the 3D step model added as shown below-

Use the Shift+right mouse button to rotate the 3D models and Ctrl+right mouse button to zoom in/out.

In order to align the two 3D bodies, go to View>Workspace Panels>PCB>PCBLIB Inspector as shown-

Then select the step model 3D body that was added and information about the body will appear in the PCBLIB Inspector panel as shown-

Now we can perform rotation of the 3D body by providing model rotation angle. Here in this case, entering 90 degree rotation angle in the model rotation X will rotate the 3D body as shown-

Depending upon the orientation you should enter the appropriate rotation angle.

To align and have a top view, go to View>Zero Rotation as shown-

Press key 2 to switch to 2D view and to see the center of the component.

Switch back to 3D view and rotate the body upside down as shown-

To align the two component together we need the center of the 3D body(step model). To mark the center of the 3D body (step model) proceed as follows. Select Tool>3D Body Placement>Add Snap Points from Vertices as shown.

Go to the one of the bottom edge of the chip and click once on the edge as shown below-

Now press Spacebar key to enter the midpoint mode. Click then again once on the same vertex and go to the opposite end vertex and click on that vertex.

Now there is a center snap point at the center of the chip.

Switch to 2D view now-

Drag the 2D part of the model with white cross center to the center of the 2D footprint so that their center align as shown-

Switch to 3D view again, the top view is shown below-

The orthogonal top view-

Go to Tool>Remove Snap Points and click on the snap points to remove the snap points.

Double click on the 3D body. This will bring up the extruded 3D body and the step model 3D body information and editing window.

Double click on the extruded 3D option, and standoff height as 0.9mm and standoff height as 0.2mm as shown below-

Double click on the generic step model editor and set the standoff height as 0.6mm as shown-

Now the final 3D model should look like the followings-

Now compile and save the integrated library project in some suitable folder.

Now bring up a new schematic sheet and place the ATMega8-16 component onto the sheet.

Now double click the component and it will bring up its properties window. Select the 32A_M footprint and you can see that the 3D step model has been added as shown below-

This completes the tutorial on adding 3D step model of ATmega8-16 in altium designer.

For more tutorials see Altium Designer Tutorials

PCB mount N connector Schematic, Footprint creation tutorial

This is a tutorial that shows how to create schematic symbol and footprint of the female N right angle bulkedge connector in altium designer. Specifically, an integrated library is created for the N connector is created using the datasheet from the manufacturer.

The N connector or Type N is widely used RF connector used to join the transceiver to the antenna using coaxial cable. It can be used for frequencies from DC to 18GHz and both 50ohm and 75ohm impedance is available. The Female N right angle bulkhead which can be mounted onto a PCB board is shown below-

The N connector used here is from the Pasternack and the model name is PE44398. The dimension of this connector is as shown-

This is a PCB mount type female N connector. It has 4 mounting hole and a center RF connector. The diameter of the mounting hole and the RF connector is 62mil. The mounting holes are separated by 400 mils.

To create an integrated library for this connector, go to File>New>Project>Integrated Library. Once done a new library package with name Integrated_Library1.LibPkg will be created. It good practice to save and rename the newly created library with some identifying name. The model name of this connector is PE44398 so here the integrated library project is saved by right clicking and selecting Save Project As and save it with name PE44398 in some folder.

To create the schematic symbol and footprint for this part we have to add a schematic library and a PCB library. To add the schematic library, right click on the PE44398.PkgLib then select Add New to Project>Schematic Library. This is as shown-

To save the schematic library with some name, 

Now we have to create a schematic symbol for this N connector. We will here simply copy the BNC connector symbol and use it for N connector. To do this, go to SCH in the bottom right corner and select SCH library as shown-

 The schematic library with component_1 will be shown on the right hand side panel. To rename this component_1, go to Tool>Rename Component and give it some name such as "PE44398".

Now open the BNC connector schematic symbol and copy the symbol as shown-

Go back to the schematic library editor for the PE44398 and paste the copied symbol into the editor as shown below-

Next we have to create the footprint and then combine the footprint to the earlier created schematic symbol.

Now to create the footprint, go back to the integrated library project panel, select and right click the PE44398.PkgLib and select Add New to Library>PCB Library as shown-

Here the footprint of the Female N right angle bulkhead will be designed. Click on the PCB Library tab visible in the left buttom(as shown in figure) and double click on the PCBCOMPONENT_1. This brings up a dialog box where you can specify the name for the pcb footprint part, provide height information and small description. Give it a name like PE44398, height of 990mils(see dimension diagram) and give a description "Female N Right Angle Bulkhead Connector" as shown-

Now we will draw the footprint for this N connector.

Notice the origin shown as a circle with cross-

Now to draw the mechanical mounting part, click on the Place Pad icon in the top toolbar. A pad will attached to the cursor. Bring it to the origin and press the tab key

This will bring up a dialog box where we can enter the value for mounting drill hole and the pad size. Enter 62mils for the hole size, 130mils (X and Y) for the pad diameter and designator as 2(designator 1 will be used for the RF connector pin later on). Refer to the datasheet/diagram of the part provided above. This is shown below-

 As soon as the pad is placed at the origin, a new pad will be attached to cursor. The new pad has to be placed 400mils to the right from the origin. Also press tab key and change the designator to 2(all mounting pad has designator 2). Go to the right by 400 mils and place the second mounting pad as shown-

As this second pad is placed another pad will be attached to the cursor, press tab key again and assign 2 as designator, go 400 mils vertically up and place it there. Similarly for the last fourth mounting pad repeat the process. After placing the 4 mounting pads the footprint will be like the one below-

Now the RF connector pin pad and mounting hole will be placed. To do this click again on the Place Pad icon, and enter the pad information. Hole size should be 62mils, pad size(X and Y) should be 90 mils, designator is 1 and placed at the center of the 4 mounting pad(refer to the part diagram). The coordinate of this pin is (200mils, 200mils).

 

To draw the outline of the part, click on Top Overlay at the bottom, then select Place Line icon and draw the rectangular outline around the pads as shown-

 Select the line tool again, go to the middle of the left line and press insert key to make it the temporary origin as shown-

From the temporary origin draw a line vertically upwards and downwards of 375mils.

Now starting from any of the tip of the new line draw a rectangle with width of 140 mils as shown-

Similarly draw the following rectangle with the provided dimension-

Select the Place by Arc Edge icon and draw an arc like the one as shown-

Drag the arc from the arc end to make it more sharp like the one shown below-

Now copy and paste the arc several times as shown-

Now we have completed the footprint for the part.

Go to the project panel again, right click on the PCB library part and select Save As to save the pcb library part with some name "PE44398" as shown-

Similarly save the Schlib1.SchLib with some name such as PE44398.Schlib as shown-

Now to give the schematic part some designator, description and add footprint information, click on the SCH Library and then double click on the PE44398 part as shown-

 This brings up the dialog box to provide information for the schematic component. For default designator type J? , provide some default comment such as N Plug Connector, provide description- Female N Right Angle Bulkedge Connector.
Then click on the Add>Footprint which is visible at the bottom of the screen of the dialog box as shown-

When the add footprint is selected, a dialog box will appear that allows us to attach the footprint. Click on the browse button, then select the footprint and click OK to attach the footprint as shown below-

Now the footprint is attached-

To add the Signal Integrity information, click on the Add Signal Integrity. In the dialog box that appears, give some model name for eg. PE44398, description- N Plug connector and select Type as Connector as shown-

The Signal Integrity is also attached now-

To complete the creation of the part as an integrated library part, go back to the project panel, select the PE44398.LibPkg, right click and select Compile Integrated Library PE44398.LibPkg to compile the integrated library project as shown

Now the new N connector part is created with integrated library that has all information- schematic, footprint and signal integrity. This part is now ready to be used.

As an example, open a new schematic sheet and browse to the library, select the PE44398.IntLib then select the part and place it on the schematic as shown-