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Insert Standard Part

Inserts library parts, such as shoulder screws, bearings, pins or bushings, on holes or shafts. The part's placement says how it goes on: SpryCAD picks the size and length and mates each part in place. One click on a face can fill its pattern, and the parts follow their faces when the parts change.

Assembly tab > Insert Standard Part.

Inserting Parts

  1. Click Insert Standard Part.
  2. Select the Part: a library part with a placement, or a family such as ISO 7379 Hexagon socket head shoulder screws.
  3. Set Fill: what a face you select fills. The default is its pattern instances.
  4. Select the cylindrical face of a hole or a shaft in the graphics area. It is added to the Faces list, and the faces it fills are highlighted. Select more faces to add them.
  5. Under Sizes, select another size for a group of faces if needed, or Flip to put the parts at their faces' other ends. The parts are shown in the graphics area as they will be added.
  6. Click OK or press Enter. The parts are added as one feature in the design tree, each mated concentric with its face and coincident with the face it stands against.
  7. Select the next faces, or click OK again with none selected, or click Close or press Esc.

Only parts and families with a placement are listed; Show all standards lists families outside the assembly's standards group too. Each OK is one step for Ctrl+Z.

On a shaft, the part stands against the shoulder, or the flat face at the end. A chamfer or fillet between them is passed over.

Retaining Rings

Select a groove's bottom face, and the ring stands against one wall. Flip puts it against the other.

Select a shaft or bore with no groove, and the ring is sized by its diameter. A Library Cut is added to the part at Groove distance from the free end, and the ring is its fitted part. The default distance meets the table's minimum edge margin, and a note warns when a distance is below it. Flip measures from the other end. To measure from a shoulder or another face, select it in Measure from, or click the planar face in the graphics area. A part in its own file is saved, after a prompt, and this cannot be undone from the assembly. An embedded part changes in this assembly only.

Faces

Fill

What each face in the list fills. Changing it changes every face in the list.

Option Fills
Its pattern instances The face and its copies in linear patterns, circular patterns and mirrors, whatever feature made it, such as a bore cut by an extrude
All holes of its Hole feature Every point of a hole's Hole feature and their copies; other faces, their pattern instances
This hole only The face alone
All holes in the part Every hole from a Hole feature in the part; other faces, their pattern instances

The Faces list names each face by its part and the feature that made it, such as Housing<1>: Cut-Extrude2, 3 pattern instances. A face picked on a counterbore stays that face, so a part can sit in the counterbore.

Right-click a face in the graphics area, or select faces in the list and right-click, to:

  • Fill its pattern instances, its feature's holes, this face only or all holes in the part, for that face alone.
  • Remove from List.
  • Skip This Hole: leave one of the faces it fills empty. Fill This Hole fills it again.
  • Flip: put the parts of the faces it fills at their other end, on top of the page's Flip.
Flip
Puts every part at the other end of its face than the family's rules choose.

Sizes

The faces are grouped by the size they take. Each group says what goes where, such as 6006 on 2 55 mm holes: its outside on the axis, its face-a against Wheel<1>, with a list of the family's rows of that size. Auto gives each face the row its rules choose. Below the groups, notes say why faces cannot take the part.

How a Part Is Placed

SpryCAD looks at each face:

  • A hole or a shaft: whether the face turns toward its axis (a hole) or away from it (a shaft).
  • Plain or tapped: a hole is tapped if it is a tapped hole from a Hole feature or has an internal Thread feature.
  • Its diameter: the size whose shoulder (or bore, or outside) fits it, within a clearance; for a tapped hole, the size of its thread.

The family's rules say which of the part's mate references goes on the axis and which stands against the face at the end of the hole or shaft. A part in a plain hole goes at the hole's mouth: the end that opens out of the part, so a bore cut from either side gets its part at its own face.

Shoulder Screws

You select The shoulder screw
A plain hole with a tapped part below it A pivot: the shoulder's end against the tapped part, the head on the hole's side. The shoulder is the length of the parts it passes through, rounded up, so the parts are free to turn
A tapped hole The shoulder's end against the face the hole opens in; the length the parts stacked over it
A plain hole with nothing tapped below The head against the hole's face; the length through the parts

A tapped part below a plain hole must have a thread the shoulder's size comes in; if not, the notes say so.

Bearings

You select The bearing
A shaft Its bore on the shaft, against the shaft's shoulder
A bore Its outside in the bore, flush with the face the bore opens in

Placing Your Own Parts

Any part in a parts library can be placed this way once it has a placement. Open the part and click Tools > Libraries > Placement:

Selection
What the part goes on: holes (plain or tapped), plain holes, tapped holes, or shafts.
Sizes
The design table whose rows are the part's sizes, or None for one size.
Matched by
The variable matched to the hole's or shaft's diameter, such as a pin's D. In a plain hole, the largest size that fits with a clearance is used; on a shaft, the size of its diameter; in a tapped hole, the size of its thread's major diameter.
Length
Optional. The variable matched to the thickness the part spans: the shortest row long enough is used.
Axis and Stop
The cylindrical face that goes on the axis, and the planar face that goes against the face at the hole's end or the shaft's shoulder. They are kept as the part's mate references.
Fit
Against the face, Flush with the face (in the hole, its stop face flush with the face), or Sunk as deep as it goes (in the hole as far as it reaches).

Then add the part to a parts library (Make Library Part). Insert Standard Part embeds it in the assembly once, with all its sizes, and configures each instance to the row it takes, so Configure changes it later.

In the Design Tree

Each OK adds a standard part feature to the design tree, such as Standard Part1. Open it to see its parts, each with a Mates folder holding the mates that hold it.

  • Double-click the feature to edit it: the page opens with its faces, family and sizes, and OK replaces what it added.
  • Right-click it for Configure Children, Appearance of Children, Hide Children or Show Children, and Suppress Children or Unsuppress Children, each for all its parts at once.
  • Delete with Its Parts removes the feature, its parts and its mates.

The parts follow their faces when the parts change, as fasteners do: see When the Parts Change.

See Also