How does the Offset Model tool work in Aspire, and what are its use cases for molds, dies, and model sizing?

Overview

Offset Model creates a 3D offset of the whole composite model: it grows or shrinks the surface by the distance you enter, like inflating or deflating the model. Unlike Scale Model Height (which multiplies the heights by a percentage), Offset Model adds or removes a consistent thickness over the surface. Its main use is making molds, dies and press tools, where a physical material thickness has to fit between a positive and a negative form. Offset Model is an Aspire tool (it has no section in the VCarve Pro manual).

How It Works

1. Make visible every component you want included. Offset Model works on the composite model (everything visible), not on individually selected components. Save the file first so you can go back.
2. Open Offset Model from the Modeling tab
3. Enter the offset distance (a positive value enlarges the model, a negative value shrinks it)
4. Tick Clip Z values to the Zero Plane if needed (see below)
5. Click Preview to see the result
6. Click OK to apply, or Cancel to exit without changes
7. Check the Component Tree after OK. You may need to hide the original components to see the offset result clearly.

Important: clicking Preview repeatedly applies the offset multiple times (it is cumulative). Check the result once, then click OK. If you have clicked Preview more than once, click Cancel, which removes the effect of all the previews, and start again.

Positive vs. Negative Offset

Positive offset: the surface grows outward by the distance. The model gets taller and each feature expands slightly.

Negative offset: the surface shrinks inward by the distance. The model gets lower and features contract. At large negative values shallow details can disappear.

Clip Z Values to the Zero Plane

After an offset, some areas of the model can end up below the zero plane. This checkbox controls what happens to them:

• Ticked: the parts that end up below the zero plane are removed, leaving only the positive values, so the final result is always positive
• Unticked: those areas stay below the zero plane

When to use it: whenever the model includes a flat plane that you do not want lowered by the offset amount. It is especially useful with a negative offset.

Fit and Tolerance Adjustment

If a CNC-cut part comes out slightly oversized, a small negative offset (for example -0.1 mm or -0.2 mm) reduces the model before you recalculate toolpaths. Treat these values as starting points and test on scrap.

Creating Matching Parts

Offset two components by equal amounts in opposite directions to create parts that nest together with a controlled gap (for example a raised panel and a matching recessed frame).

Primary Use Case: Mold and Die Making

The official documentation describes only the offset itself. The mold workflow and numbers below are examples to test on scrap, not manual figures.

When making a press mold, vacuum-forming tool or rubber mold:

1. Model the positive (master) shape in Aspire, the shape you want the finished piece to have
2. Apply a negative offset equal to the thickness of the material being formed (for example -0.03 inch for 1/32 inch material)
3. The offset model is the female (negative) mold interior. The forming material pressed between the two halves takes the shape of the original at the chosen thickness.

Example for a leather embossing die:

• Carve the positive design at 0.25 inch depth
• Apply a -0.015 inch offset so the female die leaves room for 1/64 inch leather
• Cut both the positive and the offset negative on the CNC
• Press the leather between them

Full Press-Mold Workflow (Offset Model with Add Draft)

Scenario: a finished 3D decorative medallion that you want to use as a press mold for leather, sheet metal or plastic.

Phase 1: Design the master relief

1. Finish all component work (clipart, text, background, border)
2. Use Scale Model Height if the model must fit within the mold block thickness
3. Check the 3D model in the 3D view

Phase 2: Add draft to vertical walls

1. Open Add Draft to Model and set a draft angle with the slider or the box (3 to 5 degrees is a common starting point for leather pressing, steeper for deeper vacuum forming; test on scrap)
2. Make sure only the main relief components are visible, because Add Draft bakes whatever is visible
3. Click Apply, which creates a new component named for the draft added
4. Hide the original components and keep the drafted one visible, so the walls lean outward and the formed material releases cleanly

Phase 3: Create the female cavity

For a two-part press mold (male and female halves):

1. Export the drafted model as an STL file
2. Import the STL into a new file and flip or mirror it upside down to make the female cavity shape
3. Apply Offset Model with a negative value equal to the material thickness (for example 1.5 mm leather is about -0.060 inch)
4. The offset leaves clearance between male and female that accommodates the material

For a single-sided stamp (such as a leather stamp), the drafted relief is the tool face and no female half is needed.

Phase 4: Machine the mold

1. Set up the material to match the mold blank (MDF, hardwood, HDPE or aluminum)
2. Create a 3D Roughing toolpath with a boundary
3. Create a 3D Finishing toolpath with a small stepover (try about 5 to 8% as a starting point and test on scrap)
4. Preview both toolpaths to verify coverage

Apply Draft first, then Offset

Add Draft first so there are no vertical walls, then apply Offset Model so the material thickness clearance follows the drafted surface. Doing them in the opposite order gives different geometry where sloped surfaces meet the flat base, so check the preview. For how the draft tool works, see the entry on Add Draft to Model.

Material suggestions for molds

Test a mold in foam or soft pine, and preview the toolpaths in the simulation, before cutting expensive material.

Offset Model vs. Scale Model Height