21 January 2012, by Alan
In this exercise, we will create a rotated slot that has slight clearance for a block that is to be inserted into it. The new centre-plane assembly relationship will be used to position the block.
To start with, the main part will be a 140 x 100 rectangle. The slot will cut through the part from top to bottom at an angle of 5 degrees. Using the line tool, place a line over the end face and use the connect relationship to connect the mid-point of the line to the centre of the coordinate system. Place an angular dimension on the line to ensure it is 5 degerees from the vertical.
Select the symmetric offset command:
Set the Width to 10.5mm (0.5 larger than the block to be placed) and set the Cap type to line. Click OK and pick the line just placed to define the slot.
Notice the original line now becomes a construction line. Modifying the line will modify the size and position of the slot.
Select the region inside the slot and project it back into the part by 50mm.
Save the part and place it into an assembly. The block (which is 10mm wide and 120mm square) is now placed into the assembly. A mate is used to position one face of the block to the back of the slot. For the second relationship, select the centre-plane:
The default option for selection is set to single (which is used when you can use a reference plane), but in this case we shall use the Double selection type (which uses two faces to position between). Pick the two faces of the slot to position between and then the two faces of the block:
Click OK to centre the block within the slot.
To position the block vertically, we need to edit the main part and add some angled surfaces to centre the block about. Exit the place part command, save the assembly and edit the main part. In the Pathfinder, open Used sketches, right mouse click on the sketch and pick Restore.
In the surfacing tab, select the Extruded Surface command, change the Select option to Single and pick the top edge of the slot sketch. Project back a distance and click:
Repeat this process at the bottom. This gives us the faces to position the block about. Close and return out of the part, back into the assembly.
In the Pathfinder, right mouse click on the “Show/Hide Component” and select Show Surfaces and click OK.
Click on the block in the pathfinder and select the Edit Definition button. Select the Centre-Plane relationship again and set the selection type to Double. Select the 2 surfaces just created in the main part and then select the top and bottom faces of the block to position the part.
464 total views, 1 views today