AP2257 - Draft A1 - Machined Part Modelling for CATIA V5

AIRBUS 

Procedure 

AP2257 

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: 

Authorization: 

Date : 

Name 

Function 

: Bruno Maître EMK-T 

: Head of CATIA V5 methods for French 

Team 

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 Page 1 of 46

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 

Issue:Draft A1 Date: 13 February 2002 Page 2 of 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). 

! 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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- 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. 

2.2 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 


2.5 & 5 axis 

Pocket 4 

2.5 & 5 axis 

Pockets 1 

Boss 

Stiffener 1-2 

Prismatic 

Large Pocket 

Central Stiffener 

Stiffener 3-4 

2.5 & 5 axis 

Pocket 3 

Final solid including Design 

Feature identification 

Open Prismatic 

Pocket 

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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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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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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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 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 

Sketch of Large Pocket 


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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 

workbench, make the intersection , the curve 

(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. 

Ss 

Intersection solid & (Ss) 

C 

• In a second step, project (C) on the 

reference plane (Z= 0 mm). We obtain (C1) (see 

figure ‘curve projection’). 

• The profile is defined; we can create an 

C 

extruded surface (S1) defined by the (C1) 

curve and the Z-axis. 

• 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) 

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

Curve Projection 

S1 

C1 

Offset Surface (Soff) 

distant of 0.5 mm from 

(Ss) 

Extrude Surface 

- Definition of the pocket contour 

Offset Surface 


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• 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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• 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 

• 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). 

(Ci1) 

(C1) 

Tool corner radius R = 4 

mm 

(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). 

(Ci1) 

(Cproj) 

(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 


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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. 

• 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 

L4 

L3 

0.3 

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 

• 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) 

Sketch plan 

(P1) 

(L4) 

Resources 

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

! All the geometry at this step is defined in construction mode 

• 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 

P01 

P02 

Line, Dp, of pocket 

profile 

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 (Z 

corresponding to the machining axis) 

- 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 feature with the extrude surface as one limit and the 

plan y=2mm as the other 

(Sl) 

Y=2mm 

limit 

Prismatic Pocket 2 feature 

- Constructing fillet radii 

• 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. 


R2 

Pocket bottom 

plane 

0.3 

L4 


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- Positioning of fillet radius 

• Edit the previous sketch (Sk1). 

• Add the following information : 

Circle modelling R2 tangent 

to (L1) & (L4) 

L1 

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 

- 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 

• 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 


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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 

• 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 in the PartBody. 

• 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. 


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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 

The 2 contours are 

positioned relatively via 

a concentricity 

constraint 

Positioning of boss contour 

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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• 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 


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Reference documents 

AP 2622 

AP 2610 

AP 2260 

AP 2255 

ABD 0004 

CAD layers organisation 

Naming and Numbering for New Projects 

Drawing rules for CATIA V5 

3D Modelling rules for CATIA V5 

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 

ACE/SPD/Elementary parts/ 

Mechanical Parts Generic 

CoC Structure 

EM Quality Assurance 

representative 

Approval 

C .Vergez - OIMM1 

H Schnell - ESDS 

Nicole Lamothe - EMZQ 

Record of revisions 

Issue Date Summary and reasons for changes 

Draft A1 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

AP2257 - Draft A1 - Machined Part Modelling for CATIA V5

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