3D Sketch
A 3D sketch is a run of straight lines through points anywhere in space. A normal sketch lies flat on one plane; a 3D sketch does not, so its lines can climb, turn and run off in any direction, like the bent tube of a frame or a handrail. You type each point as X, Y and Z from the origin, or pick corners of the part. Sweep can follow a 3D sketch as its path. It is one step in the Model tree.
When to Use It
- Lay out the center line of a bent tube, a roll cage, a rail or a frame that does not lie on one plane
- Give Sweep a path that turns in more than one direction, then sweep a round rod, a pipe or a profile along it
- Join corners of the part with a path, by picking them
Step by Step
- Open the model for modeling, then click Advanced on the Features tab, then 3D Sketch (on the Features tab in the other layout). The 3D Sketch panel opens with two points: P1 at the origin and P2 100 mm (4 in) up Z.
- Type X, Y and Z for each point, from the origin, in the unit shown. Empty means 0, and a minus number goes the other way. You can type any unit, like 2 in or 50 mm.
- Click Add point to add a point at the end. It goes on from the last line by the same length, so type where it really goes.
- To use corners of the part, click Pick points (it lights up), then click right on a corner of the part, a reference point or a point of another 3D sketch. Each click adds that point at the end. Click Pick points again to stop.
- Click the x at the end of a row to take that point away, or Clear to start again from two points.
- The orange line in the view shows the 3D sketch as it will be, and the line under the points says how many points and lines it has and how long it is.
- Click Make 3D Sketch. It is named 3D Sketch1 (then 3D Sketch2 and so on) and drawn as a blue line with its points.
Options
- X, Y, Z: where each point is, from the origin of the part. A picked corner keeps its exact place even though the box shows it rounded.
- Add point: a new point at the end of the run.
- Pick points: while it is on, a click adds the corner, reference point or 3D sketch point under the pointer. A drag still turns the view.
- Clear: back to two points.
- x on a row: takes that point away.
Use It as a Sweep Path
- Make the 3D sketch.
- Click Sweep. Under Path, the 3D sketch is listed with the sketches, as 3D Sketch1 (3D sketch): 3 lines.
- Pick Circular profile for a round rod or, with Thin Feature, a tube. The circle sits on the first point, square to the first line. Or pick a closed profile sketch drawn on a plane that the 3D sketch starts on or runs through.
- Click Sweep or Swept Cut. Sharp corners of the path are mitred. Sweep refuses a 3D sketch path the profile would run into itself along: two lines that cross or pass closer than the profile is wide, a turn too tight for the profile, or a line that doubles back on itself.
When you change the 3D sketch later, every sweep along it follows the new points. A 3D sketch is not offered as a guide curve, in Sweep or in Loft.
Structural members. This version has no separate Structural Member tool. A weldment member is a Sweep of a closed profile, or of a Circular profile, along a path, so a sweep along a 3D sketch is a member: Cut List lists each straight run with its cut length and mitre angles.
Edit It Later
Right-click 3D Sketch1 in the Model tree (in the Bodies group) and choose Edit Feature. The panel opens with its points. Change, add, pick or take away points and click Update 3D Sketch. Close the panel to leave it as it was.
Also on the right-click menu: Hide and Show (the line is still there for Sweep, only not drawn), Suppress, Rename and Delete. Deleting a 3D sketch that a sweep follows asks first and lists the sweeps that go with it. Suppressing it does not ask: the sweeps that follow it are suppressed with it. Unsuppress brings back only the 3D sketch, so unsuppress those sweeps after it. Making, changing and deleting a 3D sketch are each one step of Undo. The 3D sketch is saved with the part and comes back when you open it.
Tips and What to Expect
- A 3D sketch takes 2 to 100 points. For more, make a second 3D sketch.
- Two points next to each other cannot be in the same place (closer than 0.001 mm): that line would have no length.
- A point more than a kilometre (1,000,000 mm) from the origin is refused, and so is a huge typed number like 1e300.
- The lines may cross each other: the 3D sketch is still made. A sweep along it may not run into itself, so Sweep refuses lines that cross or pass closer than the profile is wide (a round rod of 2 mm needs its lines at least 2 mm apart), a turn too tight for the profile (each mitred corner needs room on the lines next to it), and a line that doubles back on itself.
- The points are numbers, frozen where they are: a picked corner does not follow the part if the part changes later.
- Honest limits: only straight lines (no arcs, splines or rounded corners), no relations or dimensions between the points, and no dragging points in the view. Only Sweep uses a 3D sketch as a path; Extrude, Revolve and Loft do not.
Common Problems
- "A 3D sketch needs at least two points. Add a point." Click Add point, or pick a corner.
- "A 3D sketch takes at most 100 points." Take some away, or make a second 3D sketch.
- "Type a number for Y of point 3, such as 25 or -12.5 (empty means 0)." That box holds something that is not a length. Type a number.
- "Points 2 and 3 of the 3D sketch are in the same place (closer than 0.001 mm), so that line has no length." Move one of them, or take one away.
- "Point 4 of the 3D sketch is more than a kilometre from the origin." Type a point nearer the origin.
- "Nothing to pick there." Click right on a corner of the part, a reference point or a point of a 3D sketch, or type the point.
- "The 3D sketch this sweep follows is gone, or comes after the sweep." The 3D sketch was deleted, or moved below the sweep in the Model tree. Move it back above the sweep, or delete the sweep.
- "The 3D sketch this sweep follows is suppressed or below the rollback bar." Unsuppress the 3D sketch, or drag the rollback bar down past it.
- "Lines 1 and 3 of the 3D sketch cross each other, and this profile needs them 2 mm apart." Sweep refuses a path that runs into itself. Move a point to keep those lines apart, or use a smaller profile.
- "The turn at point 3 of the 3D sketch is too tight for a profile this size." Make the lines next to that point longer, make the turn gentler, or use a smaller profile.
- "At point 3 the 3D sketch turns straight back: a line doubles back on itself." Move the next point off that line, or take point 3 away.
- "... cannot be read back to edit." The saved 3D sketch is damaged (more than 100 points, or a point that is not three numbers). It is never repaired quietly: delete it and make it again.