The drawer generator takes care of laying out the vectors, but there is still a little work to do before heading to the CNC. VCarve needs to know which areas to pocket, how deep to cut them, and where to cut out each piece.
This walkthrough uses the saved settings in 13in-geneator.crv, a VCarve Pro 12.510 project, as a worked example. It has two sheets, four pocket toolpaths, and two outside profiles, all using an End Mill (1/8"). Machine the pockets before cutting out the parts on each sheet. And don't forget the tabs. The small dividers need to stay put until the CNC is finished with them.
Importing the DXF
Start by downloading a DXF file from the drawer generator. Keep the material thickness used to generate that file handy. You'll need it when checking the joint depths.
Create a new job in VCarve. Set the job dimensions to match the panel you'll be cutting and enter its actual measured thickness. Use inches to match the generator. Choose your XY origin and Z-zero position to match how you'll set up the material on your CNC. I always use bottom left for my XY origin and top of material for Z-zero.
Use File > Import > Import Vectors to bring in the DXF. Vectric's vector import guide covers the import options. Check a known part dimension before going any further. Don't resize the drawing just to make everything fit on the panel; that would also change the joints.
If you need to rearrange the parts or move them to another sheet, move each outline and all of its associated pocket vectors together. Leave enough room between pieces for the profile cutter and your workholding. To reproduce the example's layout and vector selections exactly, work from a copy of the saved VCarve project; a freshly generated DXF may have different parts and positions.
The Reference Toolpaths
These are the saved operations, grouped by sheet in their machining order. Every operation starts at 0 inches. Pass depths are cumulative depths below that starting surface, not amounts to add together.
| Sheet | Toolpath name | Cut depth (in) | Pass depths (in) |
|---|---|---|---|
| 1 | Pocket 1 | 0.145 | 0.0725, 0.145 |
| 1 | Pocket 1 [1] | 0.145 | 0.0725, 0.145 |
| 1 | Pocket 1 [2] | 0.145 | 0.0725, 0.145 |
| 1 | Profile 2 | 0.270 | 0.045, 0.090, 0.135, 0.180, 0.225, 0.270 |
| 2 | Pocket 2 | 0.150 | 0.075, 0.150 |
| 2 | Profile 3 | 0.275 | 0.1375, 0.275 |
Keep these operations separate when matching the example. The three Pocket 1 operations are separate vector selections at the same depth, not three progressively deeper cuts. Profile 2 and Profile 3 also have different pass schedules; choosing the same cutter does not make their passes identical.
The reference uses 0.270-inch material on both sheets. Sheet 1 is 20.75 × 29.5 inches; Sheet 2 is 13.5 × 17 inches. Its pocket depths are therefore deeper than half the stock thickness. These numbers describe this project. For another organizer, check the generated joints and measured stock before carrying them over.
Tool Settings Used in the Example
All six operations use a 0.125-inch, two-flute end mill with tool number 3. The saved Edit Tool settings differ between pocketing and profiling:
| Setting | Pocket toolpaths | Profile toolpaths |
|---|---|---|
| Tool pass depth | 0.100 in | 0.045 in |
| Stepover | 0.050 in (40%) | 0.050 in (40%) |
| Spindle speed | 19,000 RPM | 18,000 RPM |
| Feed rate | 100 in/min | 60 in/min |
| Plunge rate | 9.5 in/min | 15 in/min |
The tool's pass-depth value does not replace the saved pass list. In particular, Profile 3 has two 0.1375-inch steps even though its Edit Tool dialog says 0.045 inches. To reproduce it, set the two passes explicitly; use shallower passes if your cutter and machine require them.
The reference also shows Safe Z at 1.0 inch and Home at X = 0, Y = 0, Z = 3.0 inches. Set these in Material Setup when matching the example, and check clearance over your workholding. The feeds, speeds, and clearances are reference settings, not universal recommendations for every machine or material.
Working Through the Layers
Open the Layers panel and look through the imported drawing one layer at a time. The reference includes names ending in _divider_dado and _shoulder, plus bottom_dogbone. These help identify the joint and corner-relief vectors. Plain part names such as front, back, left, right, bottom, and divider_1 identify outline layers to inspect for the final cutout.
Keep the outer outlines out of pocket selections. Selecting a whole panel outline for pocketing could clear away the panel you were trying to make. Inspect the dogbone reliefs too, so a missed corner doesn't stop a joint from seating.
Layers help you find the geometry; they don't require one toolpath per layer. When working from the reference project, edit each saved pocket toolpath and inspect its selected vectors before changing anything. Keep those selections to preserve the example's grouping. With a new DXF, select the corresponding joint vectors on each sheet and preview them; don't assign a depth just because a layer happens to have a similar name.
Setting the Pocket Depth
For a fresh drawer-generator layout, the nominal dado and rabbet depth is Material Thickness / 2, where T is the material thickness used in the drawer generator. For example, T = 0.25 inches gives a nominal pocket depth of 0.125 inches. This is half the material thickness, not the organizer's outside height.
To mimic the saved VCarve example, use 0.145 inches for Pocket 1, Pocket 1 [1], and Pocket 1 [2], and 0.150 inches for Pocket 2. The example therefore needs more specific guidance than setting every pocket to the same Material Thickness / 2 value. Check the fit on a sample joint when adapting those depths to your own stock.
Creating Each Pocket Toolpath
Clear any previous selection, select the intended joint vectors, and open Pocket Toolpath. Choose a 1/8-inch end mill, set Start Depth to 0 inches, and enter the appropriate cut depth from the table. Set Pocket Allowance to 0 inches and leave Ramp Plunge Moves off to match the saved operations.
Use Edit Passes to set two passes: 0.0725 and 0.145 inches for the Pocket 1 group, or 0.075 and 0.150 inches for Pocket 2. Check the actual pass list after editing the tool; the total cut depth and the tool's pass-depth setting are separate controls. Vectric's pocketing guide explains the pass controls.
Choose Offset clearing and Climb cutting. Leave Use Vector Selection Order and Project toolpath onto 3D model unchecked. Use the pocket tool settings below, then confirm the two saved passes in Edit Passes.
Calculate each operation, keep its reference name while comparing, and preview it before moving to the next selection. Check that the cutter reaches the narrow slots and corner reliefs without removing an outer panel.
Cutting Out the Pieces
Select only the outer outlines for the sheet and create a 2D Profile Toolpath with the same 1/8-inch end mill. Choose Outside / Right, use Climb cutting, and set Start Depth to 0 inches. Apply the profile feeds and speeds from the tool-settings table; they differ from the pocket settings.
For Profile 2 on Sheet 1, set Cut Depth to 0.270 inches and use six passes at the depths listed above. For Profile 3 on Sheet 2, set Cut Depth to 0.275 inches and use two passes at 0.1375 and 0.275 inches. Use Edit Passes to reproduce these schedules rather than accepting whatever the tool database supplies.
Both saved profiles use an Allowance offset of -0.010 inches. Enter the minus sign: this moves the cut into the part, making it smaller than its outline. Across two opposite straight edges, that reduces the overall size by 0.020 inches. It is an intentional difference from a zero-allowance cut, and it can affect the joints. Keep it when reproducing the reference; check a sample before applying it to a different design. Vectric's profile guide explains allowance offsets.
Leave ramps, lead-in/lead-out moves, and the separate last-pass allowance off to match the saved profiles. For your actual stock, confirm the final depth cuts through while entering the spoilboard only as much as your setup requires. A matching number alone doesn't prove the part will release.
Add Tabs
Enable Add tabs to toolpath and leave Create 3D Tabs unchecked. The reference uses flat, 2D tabs with these settings:
| Toolpath | Tab length (in) | Tab thickness (in) |
|---|---|---|
| Profile 2 | 0.500 | 0.0450 |
| Profile 3 | 0.500 | 0.0458 |
Use Edit Tabs to inspect the actual placement on every piece, especially the small dividers. Preserve the placed tabs when using the reference vectors. For a new layout, place tabs on solid sections away from joints and pocketed edges. Matching the tab dimensions alone does not reproduce their positions.
Tab thickness is measured up from the bottom of the cut depth, not from the bottom of the stock. Cutting deeper into the spoilboard leaves less wood in the tab. Check the remaining bridges in the preview after both the pockets and profiles have run. VCarve's tab placement controls let you adjust them individually.
Preview Before Cutting
Preview each sheet separately. On Sheet 1, run Pocket 1, Pocket 1 [1], and Pocket 1 [2], then Profile 2. On Sheet 2, run Pocket 2, then Profile 3. Look closely at the joints, corner reliefs, and tabs. Confirm the different pocket depths and profile pass counts, and check the size change from the negative profile allowance. The toolpath preview is a good place to catch a missed vector before it becomes a missed joint.
Save the VCarve project, then save the toolpaths using the post-processor for your CNC. Export each sheet's operations for its own stock setup, keeping its pockets ahead of its profile. Confirm the machine's XY origin, Z-zero, and safe clearance height before running the file.
Once the cutting is complete, remove the parts, trim the tabs, and clean up the edges. Then dry fit everything before reaching for the glue. A little time checking the fit now can make assembly a lot less stressful.