Parts Library
Standard stock you can drop straight into your part: square and rectangular tube, round tube, angle, channel, flat bar, round bar, square bar and plate. You do not pick from a list of every size. Drop the shape, type its sizes and its length, and it is made to those sizes. Each part you drop is a new solid body and one step in History.
When to Use It
- Lay out a frame or a stand from tube and angle without sketching each profile.
- Add a length of flat bar or a plate to a part you already have.
- Rough out a weldment quickly, then change the sizes later from History.
How to Start It
Click the narrow Library strip on the left edge of the viewer, or Library on the Features tab, to open the Library drawer. It shows a small drawing and the name of each shape. Adding parts is part of modeling, so it needs a Pro plan; on other plans the library says so and adds nothing.
Step by Step
- Drag a shape from the library onto the 3D view. Or click the shape, then click in the 3D view where it should go. With a shape clicked, Enter puts it at the origin and Esc cancels.
- A small window opens with the sizes filled in with common ones (a square tube starts at 2 x 2 in with a 1/8 in wall, 24 in long). The length box is ready to type in.
- Type the sizes you want. Any unit works ("2", "1 3/8", "50 mm", "0.125 in", "2 ft"), and fractions work. A plain number is in the units you are showing.
- Choose the way the length runs: X, Y or Z, or Edge... and then click a straight edge of the part, so the length runs along that edge. Tick Reverse direction to run the other way.
- Press Place (or Enter). The part appears as a new body, and the step is added to History. Cancel or Esc closes the window and adds nothing.
Where It Goes
- Dropped on a face of the part, it starts at the point you dropped it. When its length runs along the face, it is raised by half its size so it sits on the face rather than half inside it. When its length runs straight out of the face, it starts on the face and runs away from the part, even on a face that points down or toward the back (Reverse direction turns it the other way).
- Dropped on empty space, it goes on the ground plane (the Top plane through the origin) under the pointer, sitting on it the same way.
- The section is centred on the line through that point. The height (H, leg A, or the channel depth) points up (Y) when the length runs across; for a part standing straight up, the width runs along X.
- With nothing open yet, the first part you drop starts a new part from nothing, the same as File, New, Part.
Placing It
- While you drag, a see-through ghost of the part follows the pointer and snaps to what is under it: a corner, the middle of an edge, a point on an edge, the center of a face or of a round hole, the face itself, or the grid on the ground. A small tag says where, for example "Top face, center".
- After you drop it, the window has a Placement section. The nine dots on the drawing of the section choose the anchor: the point of the section that sits on the drop point (the center, a corner or the middle of a side). X 90, Y 90 and Z 90 (red, green and blue) turn the part a quarter turn about that axis; hold Shift to turn the other way. Flip mirrors the section, so the legs of an angle or the opening of a channel face the other way.
- X, Y and Z boxes say where the anchor goes. Any unit works and fractions down to 1/64 in ("-1 3/8", "50 mm").
- In the 3D view, drag a red, green or blue arrow to move the part along that axis (in 1/16 in or 1 mm steps), or a ring to turn it in quarter turns.
- Point to point: press it, then click a start point and an end point on the part or the grid. The part runs from the first point to the second, centered on the line, and the length is the distance between them.
- Keys: R turns again about the last axis, F flips, Tab moves the anchor to the next dot (when you are not typing in a box), Enter places, Esc cancels (during a point pick or a drag, the first Esc stops that and keeps the window).
- The placement is saved with the step, so it rebuilds the same way every time, and Edit Feature keeps the anchor where you put it when you change a size.
Options
- Square Tube and Rectangular Tube: Width (W), Height (H), Wall, Outside corner radius and Length (L). The inside corners are rounded by the outside radius less the wall.
- Round Tube: Outside diameter (OD), Wall, Length.
- Angle: Made (Hot rolled or Formed), Leg A (up), Leg B (across), Thickness, Root fillet radius, Toe radius, Length.
- Channel: Made (Hot rolled or Formed), Depth, Flange width, Web thickness, Flange thickness, Root fillet radius, Toe radius, Length. The web is on one side and the flanges run across from it.
- Flat Bar: Width, Thickness, Corner radius, Length.
- Round Bar: Diameter, Length. Square Bar: Width, Corner radius, Length.
- Plate: Width, Length (H) and Thickness. A plate's thickness runs along Y to start with, so it lies flat.
Corner Radii
Real stock has rounded corners, so the radius boxes start filled in with the typical radii for the sizes you type, and they follow the wall and the sizes until you type in one of them.
- Tube: outside corner radius 2 times the wall (the usual size for ASTM A500 tube). The inside radius is the outside less the wall.
- Hot rolled angle and channel: the heel is square, the root fillet comes from the AISC shapes table for that size (the nearest size when yours is not a standard one), and the toe radius is half the root fillet, which is an approximation.
- Formed angle and channel (bent from one sheet): inside bend radius 1 times the thickness, and the outside of the bend is the inside plus the thickness. A formed channel has one thickness for the web and the flanges, and no toe radius.
- Flat and square bar: square corners to start with.
Type any radius you want, or empty the box (or type 0) for a square corner. Reset to typical fills the boxes in again. A radius too big for the part, below zero, or not a number is refused with a short note saying why. The radii are kept with the step, so changing them later in History rebuilds the part with the new ones; in Edit Feature, Typical radii fills them in from the other sizes.
Changing It Later
The step is named after the shape and its sizes, for example "Square Tube 2 x 2 x 0.125 x 24 in". Double-click it in History (Edit Feature) to change any size or the length, then press Apply. The direction stays; a part that sat on a face is raised again for its new size. Undo, suppress, delete and dragging the step to another place in History work as they do for any other body step.
Tips and What to Expect
- Each part is always its own body, even where it touches or overlaps another body, so it never joins anything by itself. Use Combine to join bodies.
- The body is named after the shape (Square Tube 1, Square Tube 2 and so on); rename it in the Model tree if you like.
- The kernel checks every part against the area its sizes should give, so a part that comes out wrong is refused rather than added.
Problems
- "The wall must be less than half the width and less than half the height": a tube with a wall that thick would have no hole. The same goes for a round tube's wall against half its diameter.
- "The thickness must be less than both legs" (angle), and "The web thickness must be less than the flange width" or "The two flanges together must be thinner than the depth" (channel).
- "Every size ... must be more than zero", or a size over 100 metres: type a real size.
- "The toe radius must be no more than the thickness", "The root fillet and the toe radius together must be less than the inside length of the shorter leg", or "The outside corner radius must be less than half the width and half the height": the radius is too big for that size. Make it smaller, or press Reset to typical.
- "Adding parts from the Parts Library is part of modeling, which comes with Pro": the plan does not include modeling.
- "That edge is not straight": pick a straight edge, or choose X, Y or Z.
- The library does not add parts inside an assembly, to a 2D drawing, or to an older version of a file.