LAST CHECKED:
October 29, 2026


Emil Rindell

Jonas Bryntesson

Henrik Andersson
PUBLISHED:
2022-05-19

Emil Rindell

Jonas Bryntesson

Henrik Andersson
2022-05-19
In this post we will go over how to quickly export a surface to DXF. Many times you want to be able to quickly send, for example, a sheet metal for laser cutting - directly from the 3D scene without having to first create a 2D drawing .
We'll start with a short video describing what the tool does.
Face To DXF is a feature in ICMechanical (included for those with a support agreement) that allows you to export a surface directly from the 3D scene to DWG or DXF format. Many people use this feature on a daily basis, but few are aware of how to influence what actually ends up in the exported drawing file. Read on for an explanation!
Using the Face To DXF tool is very simple. Here we demonstrate the feature on an unfolded sheet metal part, but you can of course use the feature on other faces as well. Start by unfolding your sheet metal part by right-clicking it and selecting Unfold. Then go to the ICM Tools catalog, hold down the left mouse button on the Face To DXF icon, and drag and drop the feature onto the face.

You will now first be presented with a dialog box where you can choose where the DXF file should be saved. A file name is automatically suggested based on certain pre-set properties, but you can of course enter any file name you choose.
Afterwards, a presentation of what the DXF file looks like will appear. The DXF file is always exported in a 1:1 scale and is ready to be sent straight to production. However, not all the information included in the drawing file may be relevant. Read on to see how to configure the data written there.

"If I have a part with subsidence or other height differences, can I still use Face To DXF?"
Of course! If you instead hold down the right mouse button and drag-and-drop the Face to DXF icon onto the surface, a tool window will open where you can select multiple surfaces.
Here, you hold down the [Shift] key and click on the other surfaces to include in the export. Alternatively, you can choose to automatically select multiple surfaces:
Select Faces on Active Part
Settings

Right-drag the Face To DXF tool onto a surface and go to the Settings tab (the settings can also be accessed via the Windows Start menu > IronCAD Mechanical > the IPROSettings program, Utils tab).
At the top, the control of the filename and how it is assembled is shown. By default, the name in the tree(Part Name) is used. But it can be a combination of Part Name, Part Number, Description and Quantity. The Separator Character menu is used to set a character that separates these values, e.g. a space, dash, underscore, etc. The value None is the default setting and does not provide a separator. NOTE! This(None) means that the last word of one value will be written together with the first word of the next value - to one and the same word. If you use more than one value, be sure to also choose a character to separate them.

Here we find all settings for what should be written to the DXF file.


Add Material Name and Thickness to FileName - Adds the material name and sheet thickness to the file name.


Write the Thickness into the Drawing - Adds the sheet thickness as a text box in the exported DXF drawing.


Write the Code into the Drawing - Adds the material code as a text box in the exported DXF drawing.


Write the SM Material into the Drawing - Adds the material name as a text box in the exported DXF drawing.


Draw the Bend Lines into the Drawing - Adds the bend lines to the DXF file (green dashed for bend up and red dashed for bend down).


Write the Bend labels into the drawing - Adds text indicating the angle and direction of the bend, where Label Height is the text size in mm.


Write File Path into the Drawing - Adds the file path of the DXF file as a text box in the exported DXF drawing.


Write PartNumber into the Drawing - Adds the part number as a text box in the exported DXF drawing.


Write Description into the Drawing - Adds the description as a text box in the exported DXF drawing.


Write the PartName into the Drawing - Adds the name of the part as a text box in the exported DXF drawing.


Write BOM Quantity into the Drawing - Writes the quantity of parts with the same article number (Part Number) as a text box in the exported DXF drawing.


Export BSpline as Arcs - On some sheet metal parts, holes may not be completely round, which is correct if it is, for example, the contour of an intersecting tube at an angle to the surface. In the DXF file, these holes are drawn as BSplines by default. This can sometimes cause issues during laser, plasma, or waterjet cutting, as preparation software may not be able to read BSplines or handles them poorly. By enabling this function, which is active by default, the BSpline curves are converted to circular arcs instead, which all preparation software can read. The downside, however, may be a slight deviation from the exact shape ("arc").

Write Only FileName (no Path) - Outputs the file name (without the actual path) as a text box in the exported DXF drawing.


Export Face Area and Range - A text file is created alongside the DXF file, specifying the surface area and the total perimeter of the sheet metal.


Character Height for Labels in Drawing - Controls the size in mm of the text in the text boxes within the exported DXF drawing.

Use Export Path - Here you can choose to always export all files (created via Face to DXF) to a single, designated file path.
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