How to create 3D model from legacy 2D drawing using Solid Edge Create 3D command?
SolutionYou can use the Create 3D command to create dimensioned sketches in a part, sheet metal, or assembly document from 2D drawing geometry in a draft document. You can create a new model from the sketches, and you can add sketches to an existing model.
This can be useful when;
1. You have legacy 2D drawings for which you need a 3D model.
2. You want to update a 3D model with the manufacturing dimensions on a drawing.
When you select the Create 3D command, the Create 3D dialog box guides you through the process of Adding geometry and dimensions to a new model document.
Adding geometry and dimensions to an existing model document.
Will see how you can use Create 3d command, You need to import the 2d drawing file in Solid Edge using draft template.
- Go to Tools menu and select Create 3d command
- In Create 3d command select 'Add to new file' option
- In File: Browse and select which part template you want to use to create 3D part. I am using standard i s o metric part template.
- Click next > In view properties Fold principle views will be a default and active option selected
- You can change the Scale; I am keeping the scale as 1 as my 2d drawing has view scale 1 as to 1
- In Primary view orientation I will drop down select Front view to define front view for my 3d model
- Drag window select to my front view in graphics area; click next.
- Drag window select to my Right view in graphics area, click Set Fold Line.
- Define a views fold line of extreme right edge of front view to fold the right view along it.
- Click next; then click finish.
- It will take you to the part environment with the sketches you defined as front view and right view for your 3D model.
- Drag select the right view and move selecting the mid point of edge to the end point of edge in front view
- Save and close the part document. From your 2d drawing and click Create 3d command again to define top view for the 3d model.
- This time you need to select; Add to existing file.
- Browse and select the part file you just saved as your 3d part. Click; Next.
- Dropdown and select; Top view in Primary view orientation.
- Drag select the Top view sketch in graphics area and click; Next. Click; Finish.
- It will take you to the part environment again where now you have sketches for both view that is Front; Right and Top view
- Select the sketch for top view and move using steering wheel to align perfectly with the front view; check and confirm that you got correct sketches for each view
- Using Synchronous modeling; just select Extrude and select all region of top view sketch except two holes; select the direction and define length to extrude.
- Do the same for right view as demonstrated here.
- Now create a new plane using normal to curve option and select this edge to place the plane
- Go to Sketching; lock the just created plane using function F3
- Select Project to Sketch and select sketches from Top view to create region to extrude
- Once the sketch is ready on inclined plane; Select Extrude command, select the region and select extent type through next.
- Draw a concentric circle sketch of diameter 39 on the same inclined plane. Use the region and do extrude cut till 50 mili-meters.
- You can use the Create 3D command to create dimensioned sketches in a part, sheet metal, or assembly document from 2D drawing geometry in a draft document. You can create a new model from the sketches, and you can add sketches to an existing model.
- To do the last cutout you need to create close region by creating just one line sketch. Select the region and do Extrude cut symmetrical in bot directions using through all extent type option.
- That's all; your 3d model is ready; just hide all sketches, planes and P M I.
-Save the part document.