Objects in CAD

Tutorial:
Solid Edge Origin
Written By Alistar Dean

What we've done is provide a guide to the 2D to 3D process below which looks at a few different subjects than the tutorial included on the CD. It would be advisable to work through that one first and then take a look at ours. The source files can be obtained by following the link below.

source DWG (tutorial.dwg) final Solid Edge part (tutorial.par)

NB: If you should come unstuck and can't find a particular command then don't forget the tooltips which appear at the cursor as you float it over an icon or look at our icon guide.

1. Import + tidy up

a) Import: The first stage is to get your 2D AutoCAD data into the system. Its good practice to remove any extraneous entities form the drawing, such as title block, unwanted dimensions etc. You really just need the drawing entities and the critical dimensions.

The entities you need to extract from the imported AutoCAD drawing.

b) You select Open from the file menu, locate the appropriate directory and set the file type to AutoCAD (*.dwg). Before you click OK you need to set the units to millimeters in the Options. The program will then ask you what Solid Edge model type you want to use. For 2D you use the Normal.dft, which inserts the AutoCAD drawing into a blank 2D draughting sheet.

c) You now select all of those profile lines from the side view and the centre line and copy them into the clipboard (Edit/ Copy).

2. Into the third dimension

a) You now need to start up a new 3D Part window, by hitting CTRL+N for File>New, you then select Normal.par (default for a single 3D part file) from the list provided. This will bring up the part-modelling window and you're presented with the standard tri-plane co-ordinate system.

b) To start off building the 3D geometry, you need the first feature - in this case a revolved one. To create this you select the revolve icon (third down from the top on the left-hand toolbar) and choose a plane, which will be the XY in this case. This will open a new profile-sketching window. You now paste in the entities from the draught using Paste from the Edit window. You probably won't be able to see the inserted lines, so use Fit from the View menu.

c) The next stage is to define the parameters and constraints for the profile and locate it within the model space. The best way to do this is to use the Parameter assistant available from the Tools/Dimensions menu. You draw a window around the parts and click on the green arrow, you then have to click on the lower and extreme left lines to define the horizontal vertical origin for the dimensions. This will then insert the dimensions and constraints required. The system then asks you to define the axis of revolution, which is the lowest line (separate from the rest).

d) NB It may also be worth connecting the axis of revolution to the plane which is 'end-on' to the one that you're working on. To do this you just need to find the icon for Connect, select the plane line in the window and the lowest horizontal entity in the drawing, and the whole profile should shift downwards.

The appearance of the imported profile after you apply the Relationship Assistant

e) Once you have defined everything, you click the Finish button, and that'll take you back to the 3D modelling window. In the ribbon bar above the modelling window you see that you have a space to fill in the degree of revolution, you can either type in 360 or use the Revolve 360 icon. Click on finish and there you have it, you're the basics of your first 2D part.

3 Adding holes

a) To make your life a great deal easier, Solid Edge includes very useful hole creation wizards, so lets add one. To kick this off, you need to select the hole icon from the left hand toolbar. To define the hole type you want to add, you open the Hole Properties dialogue using the first icon on the new ribbon bar. In this you can define plain bores, counter sink, counter bores and counter bored holes, with a variety of threads (metric or imperial). In this case we just need a counter bored hole to accommodate a M10 socket head bolt. A quick look at the Machinery's Handbooks shows that you ned the following parameters entered into the dialogue box.

Hole Diameter: 10mm
C'Bore Diameter : 16mm
C'Bore Depth: 10mm

To define the depth you click the extent tab at the top of the box and select Through All.

The hole definition dialogue box

b) The system now returns to the model window and asks for a planar surface onwhich to place this hole. Select the fron tof the part and it then switches to a profile window in which you can place the place. As you place the hole you should align it with the vertical centre line of the first feature, then assign a dimension of 65mm between the hole centre and the centre of the first feature. A click on Finish places the hole. But a single hole will not fix this part properly. Now you're going to use the pattern icon to place 3 copies of the hole aorund the part, using the center of the first feature as a reference.

c) Firstly you need to create a pattern sketch. Click the sketch icon on the left hand toolbar and select the front face of the part and orient it as you did in the last section. Now you click the Polar Pattern icon. This brings up a new ribbon bar at the top of the screen. In this you specify the number of instances (in this case and then you draw the pattern guide by clicking on the centre of the part and then on the centre of the existing hole - Finish to place the sketch.

The Pattern Sketch for the placement of hole copies

d) The last stage is to place the hole pattern. You need to click the pattern icon from the left hand toolbar. The systemn then asks for the feature to be included, that's the hole, once done you click the green arrow. You then need to make sure that the Select from Sketch icon is depressed in the pattern ribbon at the top of the screen. You then select the pattern sketch created in 3a and hit the green arrow. A preview of the part is shown and you select Finish to place the pattern.

The final part

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