AIRBUS Machined Part Modelling for CATIA

AP2257

AIRBUS Procedure

Machined Part Modelling for CATIA V5

SCOPE: This document is relative to the modeling and know-how rules necessary with CATIAV5 to design a complex 5 axis machined part, including manufacturing needs. The guide contains different steps to define specific geometrical machining features as 2.5 axis, 4 axis, and 5 axis pockets, as ribs. It describes : -

Model organization and structure data

-

Rules to follow in case of design changes : How to show and model updated parts.

Owner’s Approval:

Name Function

Authorization:

: Bruno Maître EMK-T : Head of CATIA V5 methods for French Team

Date

:

Name Function

: Ulrich SCHUMANN-HINDENBERG : Head of CAD-CAM CM (EMK)

 Airbus 2002 . All rights reserved. This document contains Airbus proprietary information and trade secrets. It shall at all times remain the property of Airbus; no intellectual property right or licence is granted by Airbus in connection with any information contained in it. It is supplied on the express condition that said information is treated as confidential, shall not be used for any purpose other than that for which it is supplied, shall not be disclosed in whole or in part, to third parties other than the Airbus Members and Associated Partners, their subcontractors and suppliers (to the extent of their involvement in Airbus projects), without Airbus prior written consent.

Issue: Draft A1

Date: 13 February 2002

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AIRBUS Machined Part Modelling for CATIA V5

Table of contents 1

Introduction ............................................................................... 3

2

General recommendations....................................................... 4

2.1

Applicable rules ......................................................................................... 4

2.2

Practical advice.......................................................................................... 5

3

General modelling process ...................................................... 6

4

Detailed modelling process per type of difficulty ................ 20

4.1

4 or 5 axis pocket with closed angle...................................................... 20

4.1.1

Producing 2.5 axis pocket................................................................................ 20

4.1.2

Solid definition of 5 axis pocket ...................................................................... 24

4.2

4 or 5 axis pocket with open angle ........................................................ 29

4.2.1

Producing 2.5 axis pocket................................................................................ 29

4.2.2

Producing sloped pocket (4 - 5 axes).............................................................. 34

4.3

Top of stiffener modelling....................................................................... 38

4.4

Boss modelling ........................................................................................ 40

5

Identifying modifications........................................................ 44

5.1

Differences between solids made by layer ........................................... 44

5.2

Difference between solids made by 3D modelling comparison.......... 45

Reference documents ........................................................................................... 46 Group of redaction ................................................................................................ 46 Approval ................................................................................................................. 46 Record of revisions ............................................................................................... 46

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1

Introduction The aim being to: - Obtain exact geometry of the detail part, - Check and validate assemblies, - Facilitate modifications to geometry (design and production), - Avoid recreating additional geometry during the Numerical Control programming phases (the programmer will as far as possible use the solid defined by the Design Office as a basis). The method deals with general cases. Specific cases will be dealt with during CDBT meetings. For all definition principles relevant to: - Mean/nominal dimensions, - Major Definition Characteristics, - Drawing set integration (furnishing).

! !

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Consult AP2255, 3D modelling rules for CATIA V5. Consult AP2260, Drawing rules for CATIA V5.


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2

General recommendations

2.1

Applicable rules - Modelling is done in CATIAV5 exact solid form (PartDesign Workshop). The resulting model is a CATPart. Reminders: The intermediary geometry is created by means of sketches and elements obtained from the WireFrame & Surface Design workshop. The main contours bear on defined functional references such as the 3 main planes of the part (XY, ZX & YZ planes). - For parts taken from blanks, modelling must include the draft angles for the sections of the part not machined (by rework of supplier's contractual drawing). - The bores are modelled. - The threads and tapings are modelled by standard "holes" features: • to nominal diameter value for a thread, • to drilling diameter value for a tapping. -

Definition of spot facings: Use the "hole" "counterbored" feature

-

Positioning reference system

The part is modelled in its absolute axis system inside the CATPart modelled by the 3 main planes (XY, ZX, YZ). -

The curves and surfaces from the SRG (Shape reference group) are defined in the CAD model. These elements have a property giving the reference of the basic GRF file. Before any construction work, the validity of the curve or the surface from the SRG must be checked. If the size of the surface is insufficient, a new reference must be requested from the SRG.

-

Abundantly use names and explicit comments during CATIA entity creation (right click on preselected entity + properties + feature properties).

-

For the definition of a feature, perform the Boolean operations at latest possible stage in the history in order to be able to change more easily, during a modification, the topology of the latter. On completion of construction, there must be only one PartBody. Integration of restrictions is not dealt with here.

-

The construction elements will be located, if possible, on the drawing reference planes. Whenever possible, they must belong to sketches positioned on these planes. These elements will be constructed as and when the designer needs them.

-

Pockets will be modelled by the "pockets" features even for non-canonical shapes and this with the aim of optimising recognition of native features proposed by CATIA V5 in the machining workshop.

-

In a "Multi-body" approach, always prefer modelling of 2 bodies for a pocket; one body containing the definition of the pocket without fillets "assembled" with a body containing the fillet radii. This with the aim of more easily integrating the pocket bottom restrictions.

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2.2

-

Parameterising will be done by constraints on a sketch. Caution: all elements used in the current sketch must be defined in this current sketch or on a coplanar sketch plane. They must not be taken from surface elements external to the latter.

-

Do not create auxiliary co-ordinate systems (Reference axis) used for the positioning of the elements required for the construction of the part.

Practical advice -

When you modify an object (adding a fillet radius to a body), do not forget to activate the "Define in work object" command (Mouse Key 3).

-

When you want to delete an entity, take care not to destroy the parents but only the element in question. Deleting the parents is to be prohibited when the work of the definition phase is well under way.

-

The fillet radii of the walls of a pocket must not be defined on the sketch but as "fillet" features.

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3

General modelling process The modelling method of the part illustrated below includes various machining particularities. - 2.5 axis pocket - 4 or 5 axis pocket with closed angle - 4 or 5 axis pocket with open angle - Increase in stiffener height Prismatic Pocket 0.3 2.5 & 5 axis Pocket 2

Prismatic Pocket 0.2

Prismatic Pocket 0.1

2.5 & 5 axis Pocket 4

2.5 & 5 axis Pockets 1

Boss

Prismatic Large Pocket

Stiffener 1-2 Central Stiffener

Stiffener 3-4 Open Prismatic Pocket

2.5 & 5 axis Pocket 3

Final solid including Design Feature identification Step 1: Recovery of data on which part design will bear. Consists in grouping all of the resources used for the definition of the part and the Part, which will contain the definition of the part itself.

Pipe element Outside surfaces

Design Resources

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AIRBUS Machined Part Modelling for CATIA V5 Step 2:

Creation of the outside contour of the part directly on a sketch positioned on one of the main planes of the Part.

External resources required for the definition of the part. Here, visualisation of the surfaces is used only to correctly position the contour

Definition of external contour

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Step 3: Generation of the main solid (pad feature) from the contour. The fillet radii are created after generation of the prism. Group fillets with same definition by multi-selection. Prefer edge selection mode.

First definition of main In case of non-evolution profile (constant section) for pad definition, define directly the solid by surface limitation.

Surface1 used for limitation

Sketch Definition

Surface2 used for limitation

Main Solid Definition by Surfaces

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Step 4: Sculpture (split function, CATPart.

) the solid by the two surfaces referenced in the

Splitting of part body by external surfaces

Step 5: Creation of 2.5 axis pockets in "Multi-Body" approach -

Creation of the contours of the 2.5 axis pocket. •

-

Create in separate sketches but position on the reference planes the 3 sketches of the 3 pockets

Creation with 3 separate pocket features,

, 3 elementary pockets

PartBody

Body containing the 2.5 axis pockets

Pockets 0.x Definition

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The 3 elementary pockets have been assembled to comprise a body in its own right. The multi-body approach consists in separating the fillet radius entities from the bodies on which they bear. The aim of this is to facilitate later integration of the pocket bottom restrictions. General methodology for defining a pocket in multi-body approach: a- Insert a body (body1) b- Define the pocket without its radii (the body contains the sketch of the contour of the pocket and the resulting pocket feature) c- Insert a new body (body2) d- Assemble

body1 and body2

e- Activate body2 f- Define the fillet radii in body2

A body including fillets

A body containing the "raw" contour

« Multi-Body » Specification tree example

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Step 6: Subtract the upper section - Creation of an additional body. Go to main plane YZ to define sketches.

- Subtraction of the PartBody

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AIRBUS Machined Part Modelling for CATIA V5 Step 7: - 2.5 Axis Pockets 1, 2, 3 & 4 creation: •

Create common sketches for 2.5 axis pocket 1&2 and for 2.5 axis pocket 3&4 (identical transversal section) (see paragraph 4.1.1 & 4.2.1)

•

Create a new

body for each pocket

•

Define a pocket

for each one

Pocket 4

Pocket 2 Pocket 3

Pocket 1

Set of 2.5 axis Pockets without fillets - Include the different fillet with a “multi-body” modelling •

First, create the corner ones and secondly create the bottom pocket ones

- Assembly them with PartBody

2.5 Axis Pockets Assembled to the Part Body

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AIRBUS Machined Part Modelling for CATIA V5 Step 8: 5 Axis Pockets 1, 2, 3 & 4 creation: - Create one body for each 5 axis pocket - Create one sketch for each 5 axis pocket •

Create the cutting tool contour inside the different sketch (see paragraph 4.1.2 & 4.2.2)

- Create the different solid resulting from the cutting tool trajectory with slot features

5 Axis Pocket 2

5 Axis Pocket Solid

- Assembly the different bodies with Part Body

5 Axis Pocket 4

5 Axis Pocket 1

5 Axis Pocket 3

5 Axis Pocket 2

5 Axis Pockets Assembled

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Step 9: Top of Stiffeners modelling (Stiffener 1-2, Stiffener 3-4 & Central Stiffener) (see paragraph 4.3) - Creation of separate bodies, one for the stiffener 1-2, one for the stiffener 3-4 and one for the central stiffener - Create the sketches defining the material to remove on stiffener top - Create the removed solid with the loft feature

Top of Stiffener 3-4 Solid

- Assembly the 3 bodies with PartBody

Stiffeners Result on Part Body

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Step 10: - Open Pocket Modelling •

Create a specific body

•

Define the pocket contour sketch (using solid edges to construct it)

•

Define the pocket feature

Open Pocket Solid - Assembly with PartBody

Open Pocket Result

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Step 11: Adding the boss (see paragraph 4.4)

Pipe resource use

Boss in context modelling

Boss

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Step 12: Adding the 2.5 axis large pocket. - Creation of a separate body -

Pocket sketch creation using 3D definition

Sketch Plan : Z=4mm

Coincidence constraint between a 3D edge and a sketch line

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- Pocket feature creation

Feature Pocket

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-

Fillet modelling based on the ‘Multi-body’ methodology

-

Assembly with PartBody

Step 13: Final solid Adding the fillet defined on resulting surface or edge coming from boolean operation

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4

Detailed modelling process per type of difficulty

4.1

4 or 5 axis pocket with closed angle

4.1.1

Producing 2.5 axis pocket

"

Creation of pocket limit defined by a surface (S) - Definition of the pocket profile. Make the following steps in a new open body •

In

the

WireFrame

Surface

Design

, the curve workbench, make the intersection (C), between the top of part & an offset surface (Ss) of the small integral stiffener thickness (see figure ‘Intersection solid & Ss). The aim is to obtain the trace of the top part let by the cutting tool. The machining is made on 2.5 axis mode along Z. (C) on the • In a second step, project reference plane (Z= 0 mm). We obtain (C1) (see figure ‘curve projection’). •

C

Ss

Intersection solid & (Ss)

C

The profile is defined; we can create an

extruded surface curve and the Z-axis.

(S1) defined by the (C1)

• Define an offset surface (S1off) from (S1). The distance between the 2 surfaces is equal to 0.5 mm. This overthickness allow to let material to remove for the 5 axis machining (see paragraph 4.1.2)

C1 Curve Projection

S1

# (S1off) will be used to limit the pocket.

Offset Surface (Soff) distant of 0.5 mm from (Ss)

Extrude Surface

- Definition of the pocket contour Offset Surface

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AIRBUS Machined Part Modelling for CATIA V5 • In the Part Design workbench, insert a new body • Create the following in sketch in the Z=0 mm plan

Pocket 1 & 2 section

!

The pocket 1 section is the same as the pocket 3 one. By consequence, we are going to use this sketch for the pocket 1 & the pocket 3 definition. In that way, a modification in this sketch will impact the 2 pockets

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•

Pocket Feature Definition • Create a pocket feature as follow

Pocket 1 Feature creation

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AIRBUS Machined Part Modelling for CATIA V5 •

Creation of fillet radii on the walls and bottoms of the pockets (multi-body approach: see Step 5) • Create the various fillet radii.

R=11 mm

R=20 mm

R= 4 mm (bottom of pocket) 2.5 axis pockets with fillets

•

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Assemble

the pocket with the PartBody.


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4.1.2

Solid definition of 5 axis pocket - Insert a new body. - Define a plane (P) normal to the bottom of the pocket on the centre axis of the prismatic pocket. - Define the intersection of plane (P) with the surface (S) obtained from the outer skin of the part "offset" by the value of the small integral stiffener. - Define the intersection of the bottom of the pocket with (S). - Definition of sketch.

Intersection of (P) with (S): (C)

Intersection of pocket bottom plane with (S): (Cm)

Sketch plane (P)

Intersection curves

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Definition of 5 axis pocket contour without fillets (use of constraints on the sketch)

-

• On the sketch plane (P), project the curve (C). We will bear on (Cproj) to construct the line of the tool on this plane. • Define a line parallel to the reference plane (XY) offset by the value of the thickness of the pocket bottom + offset of 0.3 mm (D). • Create a line (C1) parallel to (C) offset by the value of the diameter of the tool + 1 mm. • Define a circle (Ci1), modelling the tool corner radius, tangent to (C1) and to (D). Tool corner radius R = 4 mm (Ci1) (C1)

(C1) 17 mm from (C)

(Cproj)

Line (D) parallel to reference plane offset by 5 mm + 0.3 mm

Definition of tool side (Ci1) on (P)

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- Define a line (D1) modelling the bottom of the tool tangent to (Ci1) and perpendicular to (Cproj). For an unruled surface, construct the sweep line (Db) from (C1). (Cproj)

(Ci1)

(D1): - perpendicular to (Cproj) - tangent to (Ci1)

Definition of (D1), line modelling the bottom of the tool

Case of a surface with double curvature

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Closing of contour

(Ci1) and (D) must be defined as construction elements as they do not participate in the definition of the contour

Definition of contour

The fillet radii will be modelled outside the sketch. ☞

Refer to AP2255 – 3D modelling rules for CATIA V5.

- Creation of sloped closed pocket solid (4 or 5 axes) • From the contour (Cs) on the sketch and the curve (Cm), define a "slot" feature with: As guide curve: (Cm) As profile: (Cs)

Guide curve : Cm

Cutting tool profile : Cs

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- Relimit the solid including the 0.3 mm offset on the walls (to avoid the tool was in contact with the.5 axis wall previously machined • Create the solid relimited by 2 splits.

using PartBody surfaces

5 axis pocket

Split Surfaces

Relimiting the solid

!

Use the "split" function rather than adding a "thickness" operator. Indeed, the "thickness" operator models a prism from the selected surface. Discontinuities may appear for solids when the curvature of the guide curve is high. - Add an over thickness of 0.3 mm to avoid cutting tool contact •

Use an overthickness of 0.3 mm on 2 prismatic sections (as seen on image below) Surfaces on which overthickness is applied

Overthickness Issue:Draft A1


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- Insertion of fillet radii in multi-body approach •

To the body in progress, add fillet radii: 1- For the walls (8.5 mm radius). 2- For the pocket bottoms (4 mm radius).

- Assemble this new pocket with the PartBody

4.2

4 or 5 axis pocket with open angle

4.2.1

Producing 2.5 axis pocket -

!

Definition of section construction plane

For correct distribution of the data, create a new "OpenBody" with a specific name in which we will find all of the construction data used for the construction of the 2.5 axis and 5 axis pockets. Indeed, these elements do not directly participate in the definition of the pocket contours. They must therefore not appear in the sketch associated with the "body" defining the latter.

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•

Construct the "offset" surface (S1) from the outer surface of the part offset by the value of the small integral stiffener thickness.

•

Define the pocket thickness plane intersection curve (C2) with the small integral stiffener inner surface (S1).

•

Construct a plane (P1) normal to the inner line of the contour passing through its centre. Use here the plane (P) previously used to define the 5 axis pocket.

•

Define the intersection curve between (P1) and (S1) called (C3).

•

Construct on plane (P1) the sketch containing the construction elements used to determine the contour of the 2.5 axis pocket.


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Line of pocket in this section to be determined

(4)

L1 = Inner profile line Profile line (C3),

L2 L3

0.3

L4

R1 0.3 4.5 (Pocket thickness)

SECTION through (P1)

"

!

Necessary resources to compute the profile (C3) & (L3) (see picture above : ‘SECTION through (P1)

Indeed, we need to know the (C3) profile and (L3) lines defined in the sketch plan (P1) used to construct the tool profile Use the same sketch plan (P1) as used to define the 5 axis pocket 1

Issue:Draft A1

•

In a new open body, define the intersection between the (P1) and an offset surface (Ss1) of the small integral stiffener thickness (see picture below)

•

In the same open body, define the intersection between (Ss1) and the plan Z=4.5mm corresponding to the pocket thickness.(see picture below)


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(C3)

(L4) Sketch plan (P1)

Resources -

!

All the geometry at this step is defined in construction mode

"

Dp, the tool profile, construction (see figure ‘Resulting sketch’): •

Create a sketch (Sk1) with (P1) as support.

•

L5 coincident with (C3).

•

0.3 mm offset to obtain L2.

•

L31 coincident with L3.

•

Construction of circle with radius R1. 3 constraints are associated: tangent to L21, L31 and radius of 4 mm.

•

Construction of Dp from the 2 constraints, a direction, here, vertical and tangent to the circle of radius R1.

Offset computation to create the pocket limit surface

Compute the offset between (Dp) and L5 (equal to C3) on the pocket plane Z=4.5 mm • Trim the different element to obtain the 2 points (Po1) and (Po2) • Compute the messier between these 2 elements

# We find 0.62mm as offset distance

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L2 parallel to L5

L5 coincident with (C3)

Tool corner diameter, D=8mm

Line, Dp, of pocket profile

P01 P02

L31 coincident with (L3)

(C3)in the sketch plane

Overthickness of 0.3 mm

Resulting sketch & offset analyse

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"

Definition of pocket limit surface

Once you know the offset value, we can construct in the same open body, the corresponding offset curve in the WireFrame workbench •

Define the offset surface (Ss1’) from (Ss1) distant from the offset value (here, 0.62 mm)

-

•

Compute the intersection between (Ss1’) and the pocket plane Z=4.5 mm

•

Construct the extrude surface (Sl) defined by this intersection & Z axis corresponding to the machining axis)

(Z

Creation of pocket feature without fillets •

Create a new body

•

Use the same sketch as for the previous 2.5 axis pocket (see paragraph 4.1.1)

• Define the pocket plan y=2mm as the other

feature with the extrude surface as one limit and the

(Sl)

Y=2mm limit

Prismatic Pocket 2 feature

-

Constructing fillet radii •

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In a multi-body approach, add the fillet radii to the walls (R = 11 mm) then to the bottom (R = 4 mm)


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2.5 axis pocket including fillets (multi-body approach)

4.2.2

Producing sloped pocket (4 - 5 axes) Definition: Production of fillet radius R2 between inner profile L1 and 0.3 mm offset in relation to bottom of pocket L4.

L1 = Inner profile line

R2 L4 Pocket bottom plane 0.3

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AIRBUS Machined Part Modelling for CATIA V5 -

Positioning of fillet radius •

Edit the previous sketch (Sk1).

•

Add the following information :

L1

Circle modelling R2 tangent to (L1) & (L4)

0.3 mm from bottom of pocket

L4

Line created previously modelling the bottom of the pocket

Sketch for modelling R2

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-

Determining tool "section" •

Construction of elements (L6) & (L7) to model the cutting tool.

Φ+1 L7 = Other side of the tool


Elements to be constructed

R2 L6 = Line normal to L1 (bottom of tool)

-

Define the cutting tool contour in the same sketch (Sk1)

$ Excepted the cutting tool contour, all the geometric elements belonging to this sketch have to be defined as construction ones.

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L6

α Z plane

P1

Remark:

In cases where angle α of surface has a high variation, construct two sections at the limits of the pocket to be processed and take plane Z passing via the highest point. This is valid for an open or a closed angle.

-

Creation of sloped closed pocket solid without fillets •

Use the same methodology as in the paragraph 4.1.2, in the ‘Creation of sloped closed pocket solid’ scenario Use to define the slot feature (Cm) (see paragraph 4.1.2) as guide curve and the sketch (Sk1) as profile

-

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Fillet creation with a ‘multi-body’ methodology


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4.3

Top of stiffener modelling Definition: Create removed material on top of stiffener We will use loft functionality allowing creating rapidly non-constant profile between several sections. -

Creation of sketch sections • • •

In the WireFrame & Surface workbench, inside a new open body, create 2 planes corresponding to the loft feature thickness Insert a new body In one of the 2 planes, create a sketch defining the loft section

Sketch section

• •

Issue:Draft A1

Duplicate this sketch in a new one (In this case, the profile is constant) Change the sketch support and select the second plane


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-

Loft feature creation •

In the same body, define the loft feature using the 2 sketch

Section 1

Section 2

Sections Definition -

Loft feature assembly with part body

Result on part Issue:Draft A1


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4.4

Boss modelling Definition: Create a boss on the bottom of pocket. We will use a material "addition" methodology to construct a boss on a previously defined pocket. We will remove material by modelling the centre hole. The aim is to bear using existing resource, the tube, to create and correctly position this boss.

Set the element of the pipe used to Show mode

Definition of boss in context

-

Creation of boss without hole •

-

Issue:Draft A1

Create the intersection curve between the tube and the bottom of the pocket.

Creation of geometry without "fillets". •

Insert a new body

•

Creation of a pad feature

•

Select the bottom of the pocket as sketch plane.

•

Create the circular contour of the boss: Position the boss by a concentricity constraint with the intersection curve to dimension the thickness of the boss.

in the PartBody.


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After having positioned one in relation to the other, you can define a distance constraint Intersection curve between the bottom of the pocket and the element

Boss contour

The 2 contours are positioned relatively via a concentricity constraint

Positioning of boss contour •

-

!

Once the contour has been correctly positioned, create a 3.2 mm thick "pad".

Creation of the hole or a pocket associated with the boss

Create a hole or pocket feature according to the size of the element. This definition is related to the machining process that used later, adapted to suit a pocket or a hole. On account of the dimensions, choose to define this feature as a pocket. •

Define the contour of the hole taking position in relation to the previous sketch.

Positioning of pocket contour

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AIRBUS Machined Part Modelling for CATIA V5 •

Define a pocket feature

Definition of circular pocket

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-

Creation of "fillets" (No ‘multi-body approach) •

Assemble this new body with the PartBody.

•

Create the "fillet": See example below. For a radius greater than the height of the boss, select the "Edge(s) to keep" option after clicking on the “more” button.

Edge to be conserved

Definition of the "fillet"

93 27 44

Materialisation of the "fillet"

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5

Identifying modifications

5.1

Differences between solids made by layer

New part

The modification is identified on the new solid by an extraction at a specific layer of the main modified face or faces. All adjacent faces affected by the movement of the main face are not extracted to identify the modification.

Extracted face (new face)

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5.2

Difference between solids made by 3D modelling comparison Directly in the DMU Space Analysis, you can compare 2 solids (included in a temporally same CATProduct). The methodology supposes the previous version of solid is available. -

Construct a product including the 2 versions of solid Active the compare 2 products command included in the DMU Space analysis workbench Select the previous and the new solid and select “Added + Removed” and “solid comparison.

-

"

CATIAV5 will create “3dmap” file, a CGR file, called 3Added material” and “Removed material”. -

!

Include these files in the CATProduct

Change the graphic properties of these files. For example, choose red colour for removed material and green for added material

Solid comparison Issue:Draft A1


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Reference documents AP 2622

CAD layers organisation

AP 2610

Naming and Numbering for New Projects

AP 2260

Drawing rules for CATIA V5

AP 2255

3D Modelling rules for CATIA V5

ABD 0004

Definition dossier

Group of redaction Team Members

Company / Department

Telephone

CANO-RODRIGUEZ Pedro

Airbus España

+34 916241292

Gilles MERCADIER

EMK-T

+33 561184933

Approval This document has been approved on behalf of the following: (signatures or proof of agreement are archived together with the master document) Organization

Approval

ACE/SPD/Elementary parts/ Mechanical Parts Generic

C .Vergez - OIMM1

CoC Structure

H Schnell - ESDS

EM Quality Assurance representative

Nicole Lamothe - EMZQ

Record of revisions Issue Draft A1

Date

Summary and reasons for changes

February 2002

Initial issue

If you have a query concerning the implementation or updating of this document, please contact the Owner on page 1 Or a team member of the group of redaction For general queries or information contact: Airbus Documentation Office, Airbus 31707 Blagnac CEDEX, France

Tel: 33 (0)5 61 93 49 93 Fax: 33 (0)5 61 93 27 44

Issue:Draft A1


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AIRBUS Machined Part Modelling for CATIA

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