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Complete Drawing Editor tutorial

Draw a motor-mount plate in PlanetCNC TNG

Here is a practical look at what you can now do in PlanetCNC TNG's Drawing Editor. We will draw and dimension a rounded plate outline, build its motor mounting pattern, and test how linked features respond to a change in size.

This complete tutorial covers the drawing in Steps 1–20. Along the way, you will use layers, numeric input, fillets, sketch relations, dimension annotations, construction geometry, joined profiles, duplication, and text outlines. Each screenshot opens at its original size when selected.

Step 1: Prepare the drawing

Start with a clean drawing and enable the aids that will help you build connected, accurate geometry.

  1. Open Drawing Editor. Save any existing work, then choose File → New. New drawings use millimeters.
  2. Under Grid, enable Auto Relations.
  3. Enable Snap to Objects. In its submenu, enable endpoint, center, and midpoint snapping.
  4. Turn Auto Size off and choose a 0.5 mm grid.
  5. Choose File → Save As… and save as MotorMount_00_Start.pcdraw.
The new drawing is empty, uses millimeters, and has a 0.5 mm grid.
The new drawing is empty, uses millimeters, and has a 0.5 mm grid.

Checkpoint: You have a saved, empty drawing ready for the layer setup.

Step 2: Create the layers

Set up the layers for the complete motor-mount drawing now. In this part, we will draw on 10_PROFILE; the other layers will be used as the tutorial continues.

  1. In the Layers panel, rename the existing layer to 00_REFERENCE.
  2. Use Layers → Add Layer to create the other six layers below. Edit each name in the Layer column.
Suggested layer names and colors. Colors are optional.
LayerSuggested color
00_REFERENCEGray
10_PROFILELight gray
20_MOTOR_BORECyan
30_MOTOR_HOLESYellow
40_ADJUSTMENT_SLOTSOrange
50_POCKET_2MMGreen
60_ENGRAVEViolet or magenta

Click a color swatch to change its color. The screenshot shows magenta for the engraving layer.

Click a layer color swatch to choose a color.
Click a layer color swatch to choose a color.
The seven named layers, with visibility enabled and locking disabled.
The seven named layers, with visibility enabled and locking disabled.

Leave every layer visible and unlocked. Click the 10_PROFILE row to make it current, then save with Ctrl+S.

Checkpoint: Seven layers are ready, with 10_PROFILE selected for the outline.

Step 3: Draw the outer rectangle

Use typed corner coordinates to establish the overall size without estimating positions on the canvas.

  1. Choose Tools → Rectangle.
Choose Rectangle from the Tools menu.
Choose Rectangle from the Tools menu.
  1. In the tool panel, set Type = Corners, Reference = off, and Layer = 10_PROFILE.
  2. Enter 0,0 in Corner, then press Enter.
  3. Enter 120,80 in Opposite corner, then press Enter.
Rectangle settings: opposite corners at (0,0) and (120,80), with Reference off.
Rectangle settings: opposite corners at (0,0) and (120,80), with Reference off.
  1. Choose Tools → Select to stop drawing rectangles.
  2. Choose View → Zoom Extents.
The closed rectangle is 120 mm wide and 80 mm high.
The closed rectangle is 120 mm wide and 80 mm high.

Checkpoint: One closed rectangle, with its lower-left corner at (0,0). Leave the corners sharp for the next step.

Step 4: Round the four corners

Fillets turn the sharp corners into tangent arcs. The overall plate size will remain 120 × 80 mm.

  1. Choose Tools → Fillet.
Choose Fillet from the Tools menu.
Choose Fillet from the Tools menu.
  1. Set Radius to 8 and press Enter.
Set the fillet radius to 8 mm.
Set the fillet radius to 8 mm.
  1. Click each sharp corner once: bottom-left, bottom-right, top-right, then top-left. Each becomes an R8 corner.
Round all four corners, keeping the outer dimensions unchanged.
Round all four corners, keeping the outer dimensions unchanged.
  1. Choose Tools → Select.
  2. Click a straight side of the outline. In Properties → Name, enter Plate_Profile and commit the name.
Name the closed outline Plate_Profile in Properties.
Name the closed outline Plate_Profile in Properties.
  1. Save with Ctrl+S.

Checkpoint: The profile contains four straight sides and four R8 arcs. With Auto Relations enabled, the fillets should have added corner-radius and smooth-junction relations.

Step 5: Dimension and anchor the profile

First, constrain the remaining straight portions. Then anchor the profile and add the overall dimension annotations.

Set the straight-segment lengths

  1. Choose Edit → Deselect All, then click the middle of the bottom straight segment, away from its endpoints.
  2. In Properties → Add relation, choose Distance and click the check-mark button beside it.
Select the bottom straight segment and add a Distance relation.
Select the bottom straight segment and add a Distance relation.
  1. In the Relations panel, confirm the value is 104. It is labelled Length.
  2. Deselect, then select the left straight segment. Add Distance in the same way and confirm 64.
Bottom straight segment: Length = 104 mm.
Bottom straight segment: Length = 104 mm.
Left straight segment: Length = 64 mm.
Left straight segment: Length = 64 mm.

Anchor its position

  1. Enable Helper geometry in Properties if the nodes are hidden.
  2. Deselect, then select the tangent node at (8,0), where the bottom-left arc meets the bottom straight.
  3. Confirm that node's coordinates are X = 8, Y = 0, then add Fix.
Fix the tangent node at (8,0), where the bottom-left arc meets the bottom straight.
Fix the tangent node at (8,0), where the bottom-left arc meets the bottom straight.

Fix the node, rather than the whole profile. Keep the existing R8, Smooth, Horizontal, and Vertical relations. Check that the overall bounds remain (0,0) to (120,80) and no relation is red.

Add the overall dimensions

  1. Deselect everything. Click one vertical straight side, then hold Shift and click the opposite vertical straight side, away from their nodes. In Properties, confirm that Add dimension shows Linear, then click its check-mark button. This adds the overall width dimension, 120 mm.
Select the two vertical sides and click the check mark beside Add dimension: Linear.
Select the two vertical sides and click the check mark beside Add dimension: Linear.
  1. Drag the dimension annotation to the desired position above the profile.
Drag the 120 mm width annotation into a clear position above the profile.
Drag the 120 mm width annotation into a clear position above the profile.
  1. Deselect, then select the bottom and top horizontal straight sides using Shift. Click the check mark beside Add dimension: Linear to add the overall height dimension, 80 mm. Drag its annotation to a clear position beside the profile.
The completed profile, with the 120 mm width above it and the 80 mm height beside it.
The completed profile, with the 120 mm width above it and the 80 mm height beside it.

Confirm that the annotations read 120 mm and 80 mm, then choose File → Save As… and save as MotorMount_01_Profile.pcdraw.

Checkpoint: One closed, anchored profile, four R8 corners, the correct overall dimensions, and no red or unmet relations.

Step 6: Create the motor-pattern reference

The mounting-hole pattern will use a 31 × 31 mm reference square centered at (35,40). Its corners will locate the four holes, while its diagonal will provide a reference for the motor center in the next step.

First, choose File → Save As… and save as MotorMount_02_MotorPattern.pcdraw. This preserves the profile-only checkpoint.

  1. Make 00_REFERENCE the current layer.
  2. Choose Tools → Rectangle.
  3. Turn Reference on and set Type = Size.
  4. Enter Width = 31 and Height = 31.
  5. Enter 35,40 in Center, then press Enter.
Create a 31 by 31 mm reference rectangle centered at (35,40).
Create a 31 by 31 mm reference rectangle centered at (35,40).

You should see the square and an automatically created reference diagonal.

  1. Choose Tools → Select, click a square edge, and name the square Motor_Pitch.
Name the reference square Motor_Pitch. The diagonal connects its opposite corners.
Name the reference square Motor_Pitch. The diagonal connects its opposite corners.
  1. Deselect, click the diagonal away from its endpoints and midpoint, and name it Motor_Center_Diagonal.

Check the square's opposite corners:

  • Lower-left: (19.5,24.5)
  • Upper-right: (50.5,55.5)

Leave the reference layer visible and unlocked. Save with Ctrl+S.

Checkpoint: The plate profile is unchanged, and the drawing now includes the named reference square and diagonal. The square is 31 × 31 mm, centered at (35,40).

Step 7: Anchor and dimension the reference square

Hold the motor center in place and give the square persistent side-length relations. Fixing the diagonal's midpoint keeps the center at (35,40) while allowing the mounting spacing to change.

Fix the motor center

  1. With Tools → Select, deselect everything, then select Motor_Center_Diagonal.
Select Motor_Center_Diagonal. Its midpoint is at (35,40).
Select Motor_Center_Diagonal. Its midpoint is at (35,40).
  1. In Properties, enable Helper geometry if needed, then click the Middle row's label to select the midpoint.
  2. Confirm X = 35, Y = 40, then choose Fix in Add relation and click its check-mark button.
Fix only the diagonal midpoint. The Relations panel identifies the fixed part as Middle.
Fix only the diagonal midpoint. The Relations panel identifies the fixed part as Middle.

Fix only the midpoint, rather than the entire diagonal or square. The center stays anchored while the geometry remains adjustable.

Set the mounting spacing

  1. Deselect, then select the bottom straight segment of the small square, avoiding its nodes. Add a Distance relation and confirm 31 in the Relations panel, where it is labelled Length.
Select the bottom segment of Motor_Pitch and add a Distance relation for its 31 mm length.
Select the bottom segment of Motor_Pitch and add a Distance relation for its 31 mm length.
  1. Deselect, select the square's left straight segment, and add Distance = 31 in the same way.
The two Length relations are both 31 mm, controlling the square width and height.
The two Length relations are both 31 mm, controlling the square width and height.

Keep the existing Horizontal, Vertical, and Coincident relations. Add only missing relations and keep the reference layer visible and unlocked.

Save MotorMount_02_MotorPattern.pcdraw with Ctrl+S.

Checkpoint: The reference square remains 31 × 31 mm, centered at (35,40), with no red relations. Its center is fixed and its two side lengths are controlled by the Length relations.

Step 8: Draw the motor clearance opening

Create a circle with a radius of 11.25 mm, giving a 22.5 mm diameter, at the motor center.

  1. Make 20_MOTOR_BORE the current layer.
  2. Choose Tools → Circle.
  3. Set Type = Size and turn Reference off.
  4. Enter Radius = 11.25.
  5. Enter 35,40 in Center last, then press Enter.
Create the motor clearance circle with radius 11.25 mm at (35,40).
Create the motor clearance circle with radius 11.25 mm at (35,40).
  1. Choose Tools → Select, click the circle's circumference, and name it Motor_Clearance.
Name the circle Motor_Clearance and check its center, radius, layer, and Reference flag.
Name the circle Motor_Clearance and check its center, radius, layer, and Reference flag.

Save with Ctrl+S. Leave the circle's center unfixed; the next step will link it to the reference diagonal's midpoint and add its persistent radius relation.

Checkpoint: Motor_Clearance is on 20_MOTOR_BORE, with Reference off, center (35,40), and radius 11.25 mm.

Step 9: Link and size the opening

The circle center and reference diagonal midpoint overlap at (35,40). Select each object, then use Shift+Ctrl-click to refine that selection to the required node.

Select the two overlapping nodes

  1. Choose Edit → Deselect All.
  2. Click the circle's circumference, away from its nodes.
  3. Hold Shift+Ctrl and click the circle's center. This deselects the circumference and selects the Center node.
  4. Hold Shift and click the reference diagonal, away from its endpoints and midpoint, to add it to the selection. Keep the circle's Center node selected.
  5. Hold Shift+Ctrl and click the diagonal's midpoint. This deselects the diagonal and selects its Middle node, while keeping the circle's Center node selected.
  6. Confirm that the overlapping circle center and diagonal midpoint are both selected.
The selection contains Motor_Clearance [Center] and Motor_Center_Diagonal [Middle].
The selection contains Motor_Clearance [Center] and Motor_Center_Diagonal [Middle].

Properties should show these selected parts:

  • Motor_Clearance: Center
  • Motor_Center_Diagonal: Middle

Link their positions

  1. Choose Coincident in Add relation and click the check-mark button.
Choose Coincident from the relation list to link the selected center and midpoint.
Choose Coincident from the relation list to link the selected center and midpoint.

Set the persistent radius

  1. Deselect, then select only the circle's circumference.
Select the circumference of Motor_Clearance and choose the Radius relation.
Select the circumference of Motor_Clearance and choose the Radius relation.
  1. Add Radius and confirm its value is 11.25 in the Relations panel.
The persistent Radius relation is 11.25 mm, giving a diameter of 22.5 mm.
The persistent Radius relation is 11.25 mm, giving a diameter of 22.5 mm.

Leave the circle's center unfixed: the Coincident relation links it to the already anchored reference midpoint. Save with Ctrl+S.

Checkpoint: The opening remains centered at (35,40), with diameter 22.5 mm and no red relations. Its center is linked to the reference geometry and its size is controlled by the Radius relation.

Step 10: Draw the four mounting holes

Place a circle at each corner of the reference square. Each mounting hole has a radius of 1.75 mm, giving a 3.5 mm diameter.

  1. Make 30_MOTOR_HOLES the current layer.
  2. Choose Tools → Circle.
  3. Set Type = Size, Reference = off, and Radius = 1.75.
  4. Enter the following Center coordinates one at a time, pressing Enter after each. The radius stays at 1.75.
Mounting-hole centers and the names to assign after drawing.
PositionCenter (mm)Name
Lower-left19.5,24.5Motor_Hole_LL
Lower-right50.5,24.5Motor_Hole_LR
Upper-right50.5,55.5Motor_Hole_UR
Upper-left19.5,55.5Motor_Hole_UL
Create the four mounting-hole circles with radius 1.75 mm at the reference-square corners.
Create the four mounting-hole circles with radius 1.75 mm at the reference-square corners.
  1. Choose Tools → Select and name each circle using Properties. Click its curved outline, away from its center and the reference-square edges.
Select each small circle by its circumference and assign the matching Motor_Hole name.
Select each small circle by its circumference and assign the matching Motor_Hole name.
  1. Save with Ctrl+S.

Leave the reference layer visible and unlocked. Do not add Fix or Radius relations to these holes yet; the next step will link their centers to the reference square and make their radii equal.

Checkpoint: Four named circles, each 3.5 mm in diameter, are centered on the reference-square corners and belong to 30_MOTOR_HOLES, with Reference off.

Step 11: Hole relations

Link each mounting-hole center to its matching corner of Motor_Pitch, then link the four hole sizes. Use the overlapping-node method from Step 9 to refine each object selection to the required node.

Connect the hole centers to the reference square

  1. With Tools → Select, deselect everything, then click a hole's circumference, away from its nodes.
  2. Hold Shift+Ctrl and click the hole's center. This deselects the circumference and selects its Center node.
  3. Hold Shift and click an edge of Motor_Pitch, away from its nodes, to add it to the selection. Keep the hole's Center node selected.
  4. Hold Shift+Ctrl and click the square's matching corner vertex at the hole center. This replaces the square-edge selection with its Vertex node, while keeping the hole's Center node selected.
The selection contains Motor_Hole_LL [Center] and Motor_Pitch [Vertex 1]. Coincident links their positions.
The selection contains Motor_Hole_LL [Center] and Motor_Pitch [Vertex 1]. Coincident links their positions.
  1. Confirm that Properties shows the hole's Center and the matching Motor_Pitch: Vertex as the two selected parts. Choose Coincident in Add relation and click the check-mark button.
  2. Repeat for all four holes.

Link the hole sizes

  1. Deselect and select only Motor_Hole_LL by its circumference. Add Radius = 1.75.
Select the lower-left circle by its circumference and add a Radius relation.
Select the lower-left circle by its circumference and add a Radius relation.
Set the single driving Radius relation to 1.75 mm.
Set the single driving Radius relation to 1.75 mm.
  1. Deselect, then select all four small circles by their circumferences, using Shift to add each one. Leave their center nodes unselected.
  2. Add Equal. This should create three Equal relations linking the four radii.
Select all four hole circumferences and choose Equal to link their radii.
Select all four hole circumferences and choose Equal to link their radii.

Save with Ctrl+S.

Checkpoint: All four holes remain 3.5 mm in diameter, centered on the square's corners, with no red relations.

Step 12: Test the linked holes

Make a temporary change to confirm that one radius controls all four mounting holes, then undo it to restore the intended size.

  1. Deselect, then select Motor_Hole_LL by its circumference.
  2. In the Relations panel, change its Radius from 1.75 to 2 and press Enter.
Enter 2 mm in the driving Radius relation and press Enter to test the linked hole sizes.
Enter 2 mm in the driving Radius relation and press Enter to test the linked hole sizes.
  1. Check that all four mounting holes become 4 mm in diameter, while their centers stay on the square's corners.
  2. Choose Edit → Undo. Confirm that Radius returns to 1.75 and all four holes return to 3.5 mm in diameter.

If only one hole changes or a relation turns red, undo the test change and check the Coincident, Radius, and Equal relations from Step 11 before continuing.

Hide and protect the reference geometry

Once the test passes:

  1. Deselect everything.
  2. In Layers, turn On off for 00_REFERENCE to hide it, and turn its Lock on.
  3. Save MotorMount_02_MotorPattern.pcdraw with Ctrl+S.
After restoring the 3.5 mm hole diameters, hide and lock 00_REFERENCE and save the drawing.
After restoring the 3.5 mm hole diameters, hide and lock 00_REFERENCE and save the drawing.

Checkpoint: The four holes respond together to a radius change and return to 3.5 mm after Undo. Their positions stay linked to the reference square, which is now hidden and locked.

Step 13: Draw the lower slot

Build a rounded adjustment slot from two straight lines and two semicircular arcs, then join the four pieces into one closed outline. Its overall size will be 32 × 7 mm.

  1. Choose File → Save As… and save as MotorMount_03_Slots.pcdraw, preserving the motor-pattern checkpoint.
  2. Make 40_ADJUSTMENT_SLOTS current and keep Reference off.
  3. Draw the four pieces in the table below using Tools → Line and Tools → Arc.

For each arc, set Type = Through. Enter Start, then End, then Through, pressing Enter after each field.

After each piece, choose Tools → Select before starting the next one. This finishes the Line tool's continuing chain.

Draw the lower-slot pieces in this order. All coordinates are in millimeters.
OrderToolStartEndThrough
1Line80,12.5105,12.5—
2Arc, Through105,12.5105,19.5108.5,16
3Line105,19.580,19.5—
4Arc, Through80,19.580,12.576.5,16
Enter the lower straight segment from (80,12.5) to (105,12.5) on 40_ADJUSTMENT_SLOTS.
Enter the lower straight segment from (80,12.5) to (105,12.5) on 40_ADJUSTMENT_SLOTS.
Create the right semicircle using Arc, Type = Through, with its third point at (108.5,16).
Create the right semicircle using Arc, Type = Through, with its third point at (108.5,16).

Join the pieces

  1. With Tools → Select, deselect everything, then drag a left-to-right selection box around only the four slot pieces.
Select just the two lines and two arcs that make the lower slot.
Select just the two lines and two arcs that make the lower slot.
  1. Choose Modify → Join.
  2. Name the resulting closed chain Slot_Lower and save with Ctrl+S.
The joined Slot_Lower is one closed polyline with straight segments and semicircular ends.
The joined Slot_Lower is one closed polyline with straight segments and semicircular ends.

Checkpoint: One closed outline, 32 mm long and 7 mm high, with semicircular ends. Its bounds are (76.5,12.5) to (108.5,19.5).

Step 14: Lower-slot relations

Keep the straight sides horizontal, make the line-to-arc transitions smooth, and control the slot's size and position with relations.

Use Tools → Select. Deselect before selecting a different segment and click segments away from their nodes. Add only relations that are missing.

Keep the straight sides horizontal

  1. Select the bottom straight segment and add Horizontal.
  2. Deselect, select the top straight segment, and add Horizontal.
Select a straight segment and add Horizontal; repeat for the opposite straight segment.
Select a straight segment and add Horizontal; repeat for the opposite straight segment.

Make the junctions smooth

  1. With the slot selected, click each junction node individually and add Smooth.
The four junctions between the straight segments and semicircular ends.
JunctionCoordinate (mm)
Bottom-left(80,12.5)
Bottom-right(105,12.5)
Top-right(105,19.5)
Top-left(80,19.5)

Click each node without Shift, so only that node is selected. Use Smooth for these joined transitions.

Select one junction node and add Smooth, then repeat at the other three junctions.
Select one junction node and add Smooth, then repeat at the other three junctions.

Set the end radius and straight length

  1. Deselect, select the right curved segment, and add Radius = 3.5.
Select the right arc segment and choose Radius in Add relation.
Select the right arc segment and choose Radius in Add relation.
The right arc has a 3.5 mm Radius relation and Smooth relations at its two junctions.
The right arc has a 3.5 mm Radius relation and Smooth relations at its two junctions.
  1. Deselect, select one curved segment, then Shift-click the other curved segment. Add Equal.
  2. Deselect, select the bottom straight segment, and add Distance = 25. The Relations panel labels this value Length.
  3. Select the bottom-left junction node at (80,12.5) and add Fix to that node only.

Check that the slot remains 32 × 7 mm, with no red relations. Save MotorMount_03_Slots.pcdraw with Ctrl+S.

The lower slot with its relations in place. This view also shows overall 32 mm and 7 mm dimension annotations.
The lower slot with its relations in place. This view also shows overall 32 mm and 7 mm dimension annotations.

Checkpoint: Slot_Lower has horizontal straight sides, smooth junctions, equal-radius ends, a 25 mm straight length, and a fixed anchor at (80,12.5). The overall size remains 32 × 7 mm.

Step 15: Duplicate the upper slot

Reuse the completed lower slot to create the upper one. A precise duplicate keeps the same shape and places the copy 48 mm above the original.

Keep 40_ADJUSTMENT_SLOTS current and Reference off.

  1. With Tools → Select, deselect everything, then drag a left-to-right selection rectangle around the whole lower slot.
Drag a selection rectangle around the whole lower slot.
Drag a selection rectangle around the whole lower slot.
  1. Confirm that the complete Slot_Lower chain is selected, rather than an individual node or segment.
The complete Slot_Lower chain is selected for duplication.
The complete Slot_Lower chain is selected for duplication.
  1. Choose Modify → Duplicate. In the Duplicate panel, enter dX = 0 and dY = 48, then click Apply.
Set dX to 0 and dY to 48, then apply the duplicate above the lower slot.
Set dX to 0 and dY to 48, then apply the duplicate above the lower slot.
  1. In Properties, name the new chain Slot_Upper.
Name the new upper chain Slot_Upper.
Name the new upper chain Slot_Upper.
  1. Select its bottom-left junction node at (80,60.5) and add Fix to that node only, if it is not already fixed. Keep the copied shape relations.
Fix the upper slot anchor at (80,60.5), keeping the copied shape relations.
Fix the upper slot anchor at (80,60.5), keeping the copied shape relations.

Save MotorMount_03_Slots.pcdraw with Ctrl+S.

Checkpoint: Both slots are closed and 32 × 7 mm, with their centerlines 48 mm apart. Slot_Upper has bounds (76.5,60.5) to (108.5,67.5) and belongs to 40_ADJUSTMENT_SLOTS, with Reference off.

Step 16: Check the upper-slot relations

Duplicating Slot_Lower also copied its relations. This step only verifies the upper slot; do not add the relations again.

  1. With Tools → Select, select Slot_Upper and inspect its existing relations. Deselect before selecting a different segment or node.
Inspect the existing Slot_Upper relations copied with the duplicated slot.
Inspect the existing Slot_Upper relations copied with the duplicated slot.
Verify the copied relations and the upper-slot anchor established in Step 15.
Geometry to inspectExpected relationCheck
Bottom straight segmentHorizontalPresent
Top straight segmentHorizontalPresent
Each of the four line/arc junction nodesSmoothPresent at all four junctions
Right curved segmentRadius3.5 mm
Both curved segmentsEqualThe two end radii are equal
Bottom straight segmentDistance, shown as Length25 mm
Bottom-left junction nodeFixAnchor at (80,60.5), as checked in Step 15
  1. Confirm that Slot_Upper remains a closed 32 × 7 mm chain, with bounds (76.5,60.5) to (108.5,67.5).
  2. Check that the two slot centerlines are 48 mm apart and no relation is red or unmet.
  3. Save MotorMount_03_Slots.pcdraw with Ctrl+S.

If a check fails, review the duplication and placement from Step 15 before continuing. Do not create duplicate relations or fix the whole chain.

Checkpoint: The upper slot retains the expected relations, dimensions, and anchor position. Both slots are 32 × 7 mm and their centerlines are 48 mm apart.

Step 17: Draw the relief pocket

Create a 35 × 22 mm pocket contour with R4 corners between the adjustment slots.

  1. Choose File → Save As… and save as MotorMount_04_Pocket.pcdraw, preserving the slots checkpoint.
  2. Make 50_POCKET_2MM the current layer.
  3. Choose Tools → Rectangle, set Type = Corners, and keep Reference off.
  4. Enter 75,29 in Corner, then 110,51 in Opposite corner, pressing Enter after each.
Create the relief-pocket rectangle from (75,29) to (110,51). Its name can be entered during creation.
Create the relief-pocket rectangle from (75,29) to (110,51). Its name can be entered during creation.
  1. Choose Tools → Select, then Tools → Fillet.
  2. Set Radius = 4, press Enter, and click each of the rectangle's four sharp corners once.
Set the fillet radius to 4 mm and round each of the four pocket corners.
Set the fillet radius to 4 mm and round each of the four pocket corners.
  1. Make sure the rounded chain is named Relief_Pocket. If you named it during creation, keep that name; otherwise, return to Tools → Select, select the chain, and enter Relief_Pocket in Properties → Name.
The completed rounded relief-pocket contour between the two adjustment slots.
The completed rounded relief-pocket contour between the two adjustment slots.

Save MotorMount_04_Pocket.pcdraw with Ctrl+S.

Checkpoint: The contour is named Relief_Pocket, its overall size remains 35 × 22 mm, and it has four R4 corners with no red relations.

Step 18: Pocket relations

Set the lengths of the remaining straight segments and anchor the rounded pocket at a tangent node. Use Tools → Select and add only missing relations.

  1. Deselect, then select the bottom straight segment of Relief_Pocket. Add Distance = 27.
Select the bottom straight segment of Relief_Pocket and add a Distance relation.
Select the bottom straight segment of Relief_Pocket and add a Distance relation.
The bottom straight segment has a Length relation of 27 mm.
The bottom straight segment has a Length relation of 27 mm.
  1. Deselect, select the left straight segment, and add Distance = 14.
  2. Select the bottom-left tangent node at (79,29), where the rounded corner meets the bottom straight. Add Fix to that node only.
Fix the pocket tangent node at (79,29), rather than the original sharp corner.
Fix the pocket tangent node at (79,29), rather than the original sharp corner.

Keep the existing Horizontal and Vertical side relations, four Radius = 4 relations, and eight Smooth junction relations. Do not add Equal between the already dimensioned corner arcs.

Save with Ctrl+S.

The pocket with its size and anchor relations in place. This view also shows overall 35 mm and 22 mm dimension annotations.
The pocket with its size and anchor relations in place. This view also shows overall 35 mm and 22 mm dimension annotations.

Checkpoint: The pocket remains 35 × 22 mm, bounded by (75,29) and (110,51), with four R4 corners and no red relations.

Step 19: Optional MOTOR label

Add lettering as vector outlines on the engraving layer. This step is optional; the rest of the drawing does not depend on the label.

  1. Choose File → Save As… and save as MotorMount_Final.pcdraw.
  2. Make 60_ENGRAVE the current layer.
  3. Choose Tools → Text, with Reference off.
  4. Leave the default font selected and set Height = 4, Align = Left, and Bold / Italic = off.
  5. Enter MOTOR in Text.
The Text tool previews MOTOR on the cursor before placement.
The Text tool previews MOTOR on the cursor before placement.
  1. Move onto the canvas. The text follows the cursor.
  2. Click near (8,68) to place it. Exact positioning is not important here.
  3. Switch to Tools → Select.

Keep the label as one outline object; no conversion is needed now. Save with Ctrl+S.

Checkpoint: The entire label is inside the plate, clear of the holes, and on 60_ENGRAVE, with Reference off.

Step 20: Final drawing check

Choose Tools → Select, then Edit → Deselect All and View → Zoom Extents. Keep 00_REFERENCE hidden and locked.

Check the dimensions

Expected final drawing dimensions. All lengths are in millimeters.
FeatureExpected
Outer plate120 × 80, corners R8
Motor openingDiameter 22.5, center (35,40)
Four mounting holesDiameter 3.5, spacing 31 × 31
Two slotsEach 32 × 7; centerlines 48 apart
Pocket35 × 22, corners R4

Check the geometry

  • Nine machining contours: one outer profile, one motor opening, four mounting holes, two slots, and one pocket, plus the optional label.
  • The profile, slots, and pocket are closed, with no leftover loose pieces.
  • All geometry is at Z = 0.
  • Cutting geometry has Reference off.
  • No relations are red or unmet.

Save and reopen

Save as MotorMount_Final.pcdraw, including if you skipped the optional label. Close and reopen the file, then confirm that the geometry, layers, names, relations, and dimension annotations remain intact.

Checkpoint: The final drawing reopens with the expected geometry and dimensions, and is ready for the later CAM setup.

The drawing is complete

Starting with an empty drawing, you have created a motor-mount plate with a rounded outer profile, a centered clearance opening, four mounting holes, two adjustment slots, a relief-pocket contour, and optional lettering. The geometry is organized on named layers and saved in one editable .pcdraw file.

Along the way, you used exact coordinates, fillets, geometric relations, dimension annotations, and duplication. You tested how one radius controls all four mounting holes and reused a finished slot with its relations intact. These same techniques can help you build and revise other plates, brackets, and fixtures directly in PlanetCNC TNG.

With the final checks complete, the drawing is ready for CAM preparation. That is where you will define the stock thickness, cutting tools, pocket depth, engraving operation, and machining order to turn the geometry into a machining program.

Drawing checkpoints

Download any of the five checkpoints or the final drawing to resume at a particular stage or compare your result. Each checkpoint is labelled with its last completed step. Open these .pcdraw files in PlanetCNC TNG's Drawing Editor.

This is a tutorial drawing, rather than a mounting pattern for a specific motor.

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