In this tutorial, I will cover how to create LQFP100 package with FreeCAD 1.0
First we need to have reference datasheet. Find on the internet LQFP100 datasheet with its specification.
1. Create parameters.
Open FreeCAD and create empty file.
Select spreadsheet and create empty spreadsheet.
Click F2 and rename it to "Params"
Open "Params" and fill the spreadsheet with data from the LQFP100 datasheet
Click on the empty avg cell for given parameter, for example A1 and fill "Content" box. This should create the average of two cells, we will use this value as the typical value for the parameter.
Fill the rest of the table. You can use "Ctrl + c" and "Ctrl + v" for this.
Select cells and right click, select properties:
Select display unit and fill with mm. Do the same for fi (degrees).
Right click on Cell C2, click cell properties and fill alias for later use. I will be naming parameters as LQFP_*PARAMETER NAME* in for A1 it will be "LQFP_A1". Do the same for the rest of the parameters.
Cells with an alias field filled should be highlighted blue.
Select part design and select yellow part - general purpose part container.
Create new body.
Create new sketch in that body.
Select XY plane as the reference.
The active window should look like this:
On toolbar, select centered rectangle.
Click on center dot (XYZ = 0).
FreeCad is based on the constraints, every sketch that you draw needs to be constrained, the more constrains the better, if a sketch have some freedom of movement in other words is not enough constrained, you can modify sketch with the move of the mouse
Select horizontal distance constraint.
Click on rectangle top wall:
Click on "fx" blue function icon in pop up window.
Write expression "Params.LQFP_D", and click ok.
Horizontal distance D is constrained. The value is a reference to "Params" spreadsheet cell with an alias "LQFP_D". Now do the same for the another wall using vertical constrain.
A fully constrained rectangle should turn green.
Click escape button few times to exit sketch editor.
Highlight sketch and click the pad option.
The sketch will be extruded, by the default value of 10mm.
Change the length manually or in pad parameters.
Click on blue expression icon and type "Params.LQFP_A2".
FreeCAD shows series of transformation on the left side. The series are dependent on each other and any changes on previous operation impacts another in sequence. Now the latest operation is "Pad". Click on pad, select edges and select chamfer option.
Chamfer operation will be done on selected edges. You can see that in chamfer parameters window. Now the latest operation in our list is "Chamfer"
Create a new body and rename it (click F2).
Click on "Origin002" eye icon to make "chip_leg" local reference planes visible.
Select on right top corner cube, click "left" or "right" and create new datum plane.
As the reference plane, select YZ_Plane.
Set attachment offset in Z-direction to half of the chip width - chip leg offset.
A new datum plane should be created on "right" side wall of the chip.
Click create sketch with "DatumPlane" highlighted. Now we can draw chip leg outline. These will be "front" (F) and "back" (B) legs of the chip.
Let's draw the back leg sketch according to "detail X" and then mirror the leg to create the front legs row.
Add single point to the model and set horizontal distance to "Params.LQFP_D / 2"
Add other points as necessary to create reference, I used A2, A1, L, Lp distances. The more reference points from the datasheet, the easier is the sketch to draw, as you will need fewer constraints.
You can also use polyline to draw a shape similar to chip leg and then constrain it.
Fully constrained chip leg sketch.
Exit sketch and use pad option.
It seems that chamfer is too big. Reduce it to 0.5mm It won't break our design because body and leg are independent bodies connected in one part container. That's why we are using DatumPlane - to remove dependencies between different bodies.
Select Chip_leg as active body and select Allow Compound option, set it to true
Now select "Pad001" and use linear pattern operation.
Select direction to normal sketch axis, reverse direction, offset set to LQFP_e, occurrences 25 - leg count. Click Ok.
Now select LinearPattern on the left panel and use mirror operation. Chip legs should be highlighted.
Select transform body and change reference plane to Base XZ plane. Click ok.
Repeat this action for legs on the right and the left side of the model, as the datasheet specifies different parameters for these legs.
As the LQFP100 is symmetric. You could also use "PolarPattern" for mirroring the "chip_legs", it is next to "LinearPattern" that you used before.
Now download LQFP100 model from the internet, for example KiCad library and compare. You can import a step model by simply dragging it into FreeCAD.
Let's add a marker on top of the chip. Change active body and click on top of the chip body and create new sketch.
As we added LQFP_100 model from KiCad library, we can use it as a reference to draw the circle.
Draw a circle using the other model as a reference.
Create new sketch on the top side of chip body, and use create "external geometry tool" and select body sketch corner as a reference point.
Create circle and type offset by hand. Use reference model as necessary.
Exit sketch, select "pocket" tool with new sketch selected.
Select pocket depth, click ok and exit.
Final model:
You can always go back and modify sketches and parameters, change chamfer parameters, add more details to the model.
Have fun with the tool :)
and happy new year ^^
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