Introduction to Technical Drawings

I. INTRODUCTION TO THE SOFTWARE

II. CREATING SUPPLEMENTARY DRAWINGS

III. REFERENCE

Problem

Solution

Dimensioning appears to be incorrect.

Click inside the viewport before dimensioning. It should be highlighted in green/red.

If the dimension is still wrong and you are dimensioning added lines or circles, be sure to highlight the corresponding viewport before drawing them. Otherwise, dimensions will be wrong if your viewport has been scaled!

 The base view is not oriented properly.

Set the orientation when creating the view. After selecting "Current" for Orientation, click the small button to the right to change the orientation.

Use the Zoom All button (a square with arrows pointing out to each side) to put the object into view if it is not visible on the screen.

Cannot dimension between lines.

The lines are likely not parallel or they are not straight.

To Fix Non-Parallel Lines: In Sketch Mode, click Parallel on the Drawing Sketch Panel (it is under the drop-down menu beside Perpendicular) and select both lines. To enter Sketch Mode and edit a line, double-click that line.

To get an approximate dimension between curves (ie. a reference dimension), draw two small lines and measure between them.

To get an exact dimension, measure between the two farthest points.

Desired Effect

Action

Draw a line with a pre-determined length from a specific point.

A set point/line must exist from which you are measuring.

Enter Sketch Mode to draw a line.

Draw the desired line approximately the correct distance from the set point OR, if you are using a set line, draw the new desired line parallel to the set line. To do so, draw the desired line approximately parallel to the set line in Sketch Mode. Click Project Geometry on the Drawing Sketch and click on the set line. Finish the action. Next click Parallel on the Drawing Sketch Panel (hold on the arrow beside Perpendicular to get this option). Select both lines, then finish the action.

In Sketch Mode, create a general dimension between the desired line and set line/point and double-click to edit the dimension. Enter the desired length. Select and drag to move as necessary.

Draw a 3-Point Curve

In Sketch mode, click the 3-point curve button.

Click each edge, then one point in the middle to fit the curve.

Hide Lines/Make Lines Invisible

In the regular view, right-click the line and deselect "Visibility".

To hide hatching in a sectional view, right-click a hatch line and select "Hide Hatching".

Add Hatching

Draw the entire closed area that must be hatched in Sketch Mode

Select Fill/Hatching from the Drawing Toolbar and select the closed region. The region must be closed or it will not be selectable.

Add a Leader Head

Draw a leader as normal.

When finished, right click the leader and Add new vertex/leader

Select the surface to point to, then click the intersection point of the leaders.

Change Page Size

 Add any referenced logo to the part folder. Otherwise, when the title block definition is edited, the logo will not print with the document.

Right-click "Sheet" > Edit Sheet > Change page width as desired

Right-click "Multi" > Edit Instance > Change number of horizontal zones to fit new page size (number of pages x 8 zones)

Right-click ANSI > Edit Definition > In the title box, edit the text and correct the template size.

Key Command

Function

s

Enter/exit Sketch Mode

l

Start a new line in Sketch Mode

SHIFT + c

Start a circle in Sketch Mode

Esc

Finish the current command

Command

Feature

i) Simultaneous left & right click and hold

ii) Middle click

iii) Release buttons, and move mouse up/down to zoom in/out

Zoom

i) Middle click and hold

ii) Move mouse to pan

Pan

Rotate

To rotate around a specific point, right click that point before rotating.

To rotate the object purely clockwise or counterclockwise, rotate outside of the rotation circle. Conversely, to rotate the object towards or away from the screen, rotate inside the rotation circle.

Select "Measuring" from DMU Dimensioning toolbar.

Measure

Four measuring styles exist (three of which will likely be used). The first measures the shortest distance from the first click to the second click, then resets. The second measures the shortest distance from the first click to all following clicks (ie. always measures from the same base point). The third style can be ignored for these purposes. The fourth measuring style measures radii/diameters/fillets.

Further, different ways of selecting dimensions can be specified. Often "All geometry infinite" should be selected, but methods can sometimes be more useful. For example, a radius can be approximated by using the 3-point-arc tool, when it is impossible to measure using the other tools.

Term

Meaning

Fillet

Usually a radius connecting two surfaces.

Chamfer

A plane that intersects two other planes. Use discretion when choosing whether to dimension some non-obvious "chamfers".

Profile

The "flattened" outline of a surface when looking directly at it

(i.e. silhouette).

Stiffener

A wall that usually runs perpendicular to outside walls. Stiffeners are usually thinner than outer walls.

Basics:           

Drawings generally include 2-4 basic views (depending on complexity), all part notes, and dimensions for all other thicknesses, radii, and chamfers. The title block should include the file name, drawing name, part number, and part name. Include reference dimensions for the overall part size.

How many pages do I need?

 Estimate how many thicknesses and radii you'll need to dimension, and how many views you'll need to show part notes. One page is usually enough for simple parts; one or two may be necessary for fully-dimensioned simple parts; three pages is usually reserved for quite complex parts with many thicknesses or reserved flagnote areas. Four pages are seldom used, but it is better to err on more space than not enough room or crammed views. Technical drawings use a page size of 11" x 17".

How can I dimension thicknesses?

 If the thickness is not visible in the current view, dimension floor thicknesses with leaders, but instead of an arrowhead use a small dot to refer to a surface. If the thickness is visible in the current view (ie. a wall or stiffener thickness), dimension regularly. Many parallel dimensions can be labeled once followed by "typical" note. Alternatively thicknesses can be shown by taking a section through the desired area

How can I dimension radii and fillets?

 If corner radii are repeated, only dimension one corner and add a "typical" note. Try to dimension through the center of the radii. Rarely is it acceptable to point at a fillet to dimension it if the radius is not visible in the current view; usually a section or side view is used to show the true radius. If fillet radii are repeated, add a typical note to avoid dimensioning every fillet. Most other radii should be dimensioned individually, and always through the center of the radii when possible. See the end of the chapter for common "typical" notes.

How can I dimension chamfers?

 Show the true chamfer. If the angle is 45° and the two outer surfaces are perpendicular, point a leader at the angled surface with the note: __(CHAMFER DIST)__ X 45°

If the angle is not 45° or the surface are not perpendicular, dimension each chamfer distance individually.

Which views do I include?

 Include a "front" view of the part, flattened to the primary and secondary datum, when applicable. Show a side or top view to show the part thickness. In general, show both side views if they are not the same, and show the top and bottom views if they are not the same. The views should make the orientation of the part obvious, but not be repetitive.

How do I fully dimension a part?

First, ensure the part is "flat" to the highest ranking datum (ie. A), and also flat to the next highest ranking perpendicular datum (ie. B). By hand or using the baseline dimensioning feature in AutoDesk, dimension every part feature both horizontally and vertically from the highest-ranking datum possible. Fully dimensioning is analogous to giving coordinates from the datums, which act as reference planes (or an origin). Do not over-dimension, ie. repeat dimensions, dimension thicknesses, or add unnecessary dimensions. For example, if a fillet is adjacent to a wall, there is no need to dimension to the centre of the fillet and to the wall edge; simply dimensions to the wall, and the dimension to the centre of the fillet can be found by adding or subtracting the fillet radius.

If two perpendicular dimensions are not available, dimension to a large surface that is perpendicular to the available datum. Datums (for example, diametrical datums) can be extended on to projected views and used to dimension fully.

Prismatic parts are very difficult to fully dimension; generally the 3D model is used to describe the part dimensions.

What is a detail view and when do I use it?

A detail is used when a lot of annotations or dimensions are applied to a small area and there is insufficient room on the drawing to show the notes clearly. A detail can also be used to show hatching or highlighting more clearly, or to show -MOD holes. A detail is essentially a magnification of a small area of the part.

What is a section view?

A section is a cut through the part to show otherwise difficult to see features or thicknesses. A full section cuts the part along the section line and looks in the direction of the arrowheads at the rest of the part from that point onwards. A distance section takes a sliver of part and looks only at that sliver in the direction of the arrowheads. While, a full section is more "correct", a distance section is often clearer when showing small features and thicknesses.

What is a broken view and when do I use it? What are broken dimensions?

 A broken view is used generally on parts that have long featureless sections in the middle, but ends that require a greater magnification (ie. a pipe).

Broken dimensions are used when the center of the radius does not fit on the visible page, but needs to be dimensioned to (ie. if the part is fully dimensioned).

What are datum targets and how to they relate to regular datums?

Positional and pattern tolerances are usually referenced to datums, which are specific reference planes notes in the model. Complex parts sometimes have many datums, and often use surfaces oriented at different angles to define the datums. Datums are usually defined by a surface (ie. one line is defined by the datum) or a diameter, (in which case two lines are defined by the datum).

Datum targets are sometimes used to define datum planes. When two datum targets are given for the same datum letter (ie. B1 and B2), the datum plane is defined by the line between the targets. When one datum target is used, the datum is usually defined by the line perpendicular to the previous datum, which also passes through the target. For example, a datum target C1 may define datum C, which is the perpendicular line to datum B that runs through target C1. Complicated datums such as this are not usually included because any measurement to that datum will not be measured manually. However, when including these datums, usually a reference angle is given to a surface to show the orientation of the datum relative to the part.

Basics:           

Drawings generally include 2-4 basic views (depending on complexity), all part notes including joint and sealant definitions, joint details when applicable, and labels for all parts. The title block should include the file name, drawing name, part number, and part name. Include reference dimensions for the overall part size

How do I show sealant definitions?

 Sealant definitions are generally shown by pointing to the surface on which they apply in the part stackup. If that is not applicable or sufficiently clear, the sealant application area can be hatched to add emphasis.

When do I show a part stackup on the drawing?

 Part stackups are shown when the actual stackup is not obvious (ie. there are "hidden" washers), complex (ie. there are many components), or when a sealant definition needs to be labeled.

Another technique is to show part stackups are for all joint definitions, regardless of complexity.

What are joint details and when do I use them?

Joint details are similar to joint definitions, except that they are not marked in the 3D Catia dataset. Joint details must be added when a part stackup is complex or ambiguous (i.e. there are more components than just the nutplate, rivet, and part). Joint detail numbering generally starts at 01, rather than picking up after the last joint definition number. Joint details need not be added to the SNL because they are not extracted from the part data set.

Type

Description

Opposites

The existence of an opposite will be noted in the parts list and likely in the part data set. When an opposite part note is included in the model, make sure to include it on the SNL. A note should be added beneath the main view on the first page of the SD reading:

-1 SHOWN

-2 OPPOSITE

The naming convention for an opposite is:

Part number: 123A1234-1 (-2 OPPOSITE)

SD Number: 123A1234-1-2

File Name:

SD_123A1234-1-2_REVNC (detail or assembly drawings)

SNL_123A1234-1-2_REVNC (detail SNL)

SNL_123A1234-1_REVNC, SNL_313U1234-2_REVNC (assembly SNLs)

Remember that a detail only has one drawing and one SNL, even for opposites, while an assembly has one drawing and two SNLs for opposites.

 The first number of an assembly is usually the part authority (ie. for a 1-2 opposite set, the -1 is usually the part authority), although it should be listed in the parts list and is usually listed in the model. If the -1 is the part authority, include only the -1 original CAD and parts list information on the -1 SNL. On the -2 SNL, include both the -1 and -2 original CAD and parts list information, because the -2 is dependent on the part authority.

-MOD Configuration

 A drawing will require a -MOD configuration if holes must be drilled on the part that are not modeled on the 3D Catia model. Generally â-MOD holes are rivet holes for nutplates (which are often hidden under fastener locations or nutplate locations in the tree when the part is opened in Enovia). Sometimes, however, -MOD holes are needed to satisfy upper level assemblies, and in most of these cases they are not marked on the sub-assembly in any way.

For nutplate -MOD holes, create a detail view of the -MOD area, label the large bolt hole as reference and assign it a datum, draw the two rivet holes, and dimension them as .1030"/.0980" with positional tolerance of .0020" at maximum material condition with respect to the new datum.

 Upper assembly -MOD holes often vary based on the situation. In general, many holes over a large area will be given a pattern tolerance (with respect to each other) and dimensioned as #40 pilot holes. Fewer holes in a small area will be given a pattern and positional tolerance and probably drilled at full size.

Adding a -MOD note to the SNL to state the reason for -MOD holes is a new procedure that may be required in some cases.

Type of Tolerance

Description

Default

 No tolerance given. Use when the tolerance for this feature is already given in the SNL or parts list (ie. thicknesses).

Basic

 According to ASME 2004, a basic dimension is the theoretical exact size. According to the machinery handbook, a basic dimension is the nominal size. Use when dimensioning lengths to which the general profile tolerance does not apply (ie. fully dimensioned lengths). For most sub-contracted parts, all of the dimensions (lengths, radii, chamfers) will be basic.

Reference

No tolerance exists - use as reference only. Use when repeating dimensions that have already been given a tolerance or for full-size dimensions.

Symmetric

 Tolerance is +/- the same number (i.e. +/- .0050").

Deviation

 Tolerance is +/- different numbers (i.e. +.0020", -.0030")

Limits Linear

 The maximum and minimum acceptable values are listed horizontally and separated by a dash.

Limits Stacked

 The maximum and minimum acceptable values are listed vertically as a stack.

Problem

Solution

Part will not section

Move the view to be sectioned away from all other viewports (sometimes viewport overlap causes an error)

Try creating a section with a distance of .001 in (the default is .25 in)

If all else fails, ask for the model to be regenerated, otherwise draw the section in by hand

Some component of Assembly is outdated or corrupted

Save the new replacement .ipt file to the part folder (with a different name than the original)

Open the .iam Assembly file in Inventor and select the Replace option in the toolbar

Delete the old file from the assembly in Inventor and the part folder

Situation

Dimensioning Method

Wall of constant thickness intersected by other walls/stiffeners

Dimension only one end of the wall, in a regular view, and follow with "TYP". If not otherwise specified, continued sections of a wall are assumed to be parallel. If some sections are different thicknesses, add "TYP UNLESS OTHERWISE SPECIFIED" and dimensions walls with different thicknesses. The same labeling conventions can be applied to a section taken through the desired area.

Repeated radii on features

Several types of this case occur commonly. In all cases, dimension one of the radii, followed by the appropriate note:

• Repeated fillet radii:

"FILLET RADII"

• Repeated corner radii:

"CORNER RADII"

• Repeated external radii on some exterior surface that is not easily viewed, where the surfaces follow a similar but not exact pattern:

"EXTERNAL PROFILE CORNER RADII"

"TYPICAL FOR ALL _________ UNLESS OTHERWISE SPECIFIED"

Repeated floor thickness

Dimension once and follow with:

"TYPICAL FOR ALL FLOOR THICKNESSES

UNLESS OTHERWISE SPECIFIED"

Wall thicknesses and stiffeners can sometimes be dimensioned as typical also.

Drawing Type

Description

Other Notes

Basic Assembly

All joint definitions are matched with specific nutplates.

Label the joint definitions per rivet (ie. per hole) and show the rivet assemblies.

Complex Assembly

Joint definitions are not nutplate-specific.

Label each nutplate and create a Rivet Code table. Label each rivet according to its rivet type.

Undefined -MOD Holes

-MOD holes are not marked on detail model. Size and tolerance needs to be determined.

In general, positional tolerances for holes patterns should be applied. For few holes in a specific pattern over a small area, the full size is usually given (this can be found either in the tree in Enovia or looked up for the individual rivet/bolt size using the specified BAC). For many holes over a large space, #40 pilot holes (.1030"/.0980") will probably be used.

Simple, Fully Dimensioned, Symmetrical

Lines of symmetry can be defined in one or two axes (whichever is appropriate). Symmetry is sometimes also defined in the SNL.

Closed Angle Mismatch

Cutter ramp specified in MBD.

Label the cutter ramp section as "CUTTER RAMP" (rather than a section, i.e. SECTION A-A). Specify TYPICAL CLOSED ANGLE MISMATCH, TYPICAL CLOSED ANGLE MISMATCH EXCEPT AS NOTED, TYPICAL CLOSED ANGLE MISMATCH WHERE INDICATED, etc.

Drawing refers to a BAC

The parts list calls for the use of a BAC. Ask for a copy of the required BAC and include it in the part folder.

Include dimensions specifically requested by the BAC. Ask first to make sure you actually need to use the BAC (it will be referred to in the Components/Materials section of the SNL.