Sheet metal settings · Convert to sheet metal · 日本語 · Printable PDF (Japanese, 2 pages)
Base plate: profile, thickness and direction
1. What Base plate creates
Add thickness to one closed planar profile to create a new sheet-metal solid. Work stays in model space. The original profile remains in place. Sheet-metal information is assigned automatically, so Convert to sheet metal is not required afterwards.
2. Workflow
- Prepare one closed planar profile, such as a circle, closed polyline or closed path. Join separate segments into a closed path first.
- Open Sheet metal → Base plate.
- Under Closed profile, click Pick in CAD and select that outline. This field expects a curve object, not an existing solid or its face.
- Enter the total thickness t, using the unit shown by the input field.
- Choose Thickness direction. The schematic above switches to match your choice.
- Click Apply. Check the result, close the dialog and save the drawing.
Selecting a profile or editing values does not create a solid. Creation runs on Apply. Thickness must be positive.
3. Positive, Negative and Symmetric
| Direction | Position relative to the original profile plane |
|---|---|
| Positive | Add thickness t toward +n. The profile plane becomes one surface of the plate. |
| Negative | Add thickness t toward -n, on the opposite side. |
| Symmetric | Keep the profile plane at mid-thickness and add t/2 to each side. Total thickness is t, not 2t. |
On the usual XY work plane, Positive means up (+Z) and Negative means down (-Z). Drawing the profile clockwise or counterclockwise does not change this. Thickness direction is separate from inside/outside bend choices.
+n is perpendicular to the profile plane and oriented toward the +Z side of the work plane captured when the command starts. A tilted work plane uses its own coordinate axes. Rotating the view during the command does not swap the sides. For a profile perpendicular to the work plane, +Y is used to choose the positive side, then +X if needed. The drawing is a schematic, not a preview of the actual profile or entered dimensions.
If the plate is on the wrong side, keep the same dialog open, switch between Positive and Negative and click Apply again. The plate most recently created by this command is replaced with the new result.
4. After creation and troubleshooting
| Situation | Action |
|---|---|
| U-shaped or L-shaped plates | Concave outlines are supported when the entire boundary forms one closed loop. A polyline with coincident start and end points is accepted even when its closed flag is off. Only the working copy is closed; the original outline remains unchanged. |
| Cannot select the profile | Use one curve object forming a closed loop. Separate lines, outlines with an endpoint gap and solids are not accepted. |
| Apply fails | Check that the outline is planar and closed, with no self-intersections or invalid overlaps. |
| A plate with holes is needed | The current command takes one profile, not a simultaneous outer loop and several hole loops. Create the plate first, then make the holes with the usual cutting commands. |
| Change thickness or direction after creation | While the same dialog stays open, change the values and apply again to replace its previous result. Closing it and starting a new Base plate command creates a new plate. Undo or remove an unwanted earlier plate before starting again. |
Closed profile → Base plate → Edge flange / Bend along line → Unfold and cut → Refold
For an existing flat solid, use Convert to sheet metal instead. Creating a base plate does not create bends or reliefs.