AssemblyDesign (7) - Publication CATIA アセンブリデザイン基礎 (7)

パブリッシュについて About Publication

休日の午前中に　ハイウェイを走ると
帰りのことは考えない

*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


SECTION 1
「パブリッシュ」って何？ What is a "Publication"?
Publishing elements is the process of creating geometrical features available to different
users. Useful when working in assembly design context. For example, constraints within the
component will be kept even after a component is replaced with another.


SECTION 2
パブリッシュの作成 Publishing Elements

1. パブリッシュの作成 Publishing Elements
Go to Tools > Publication (Available in both Part file and Assembly file)
Additional Note: How to select an axis for Publication
1) Right-click on he geometry
2) Select "Other selection" from the contextual menu
3) Select "Axis" in the pop-up winodw

2. パブリッシュ名の変更 Changing Published Names
1) Go to Tools > Publication
2) In the pop-up, select (highlight) the published name you want to modify, and then click on
it one more time.

3. Others
"Remove" button
"Import" button: Text files can be imported to CATIA. Useful when elemets to publish are
determined in the group or company. (Published names can be shared with other users in the same
group or company.)
"Export" button: Published names can be exported with text format.
"Publish a face, edge, axis, vertex, or extremity" check box:


SECTION 3
パブリッシュの活用方法 Utility of Publication
Useful when creating constraints, or working with contextual data

1. Publish faces, and create constraints with them.
Replace componets, and the constraints are not broken.

2. Working with contextual data
Go to Tools > Options > Part Infrastructure > General (tab) > External Reference (area)
==> Check "Keep link with selected object".

Note: Published names will have to be assigned correspondingly

"Driving Part" consists of Sketches & surface, while "Contextual Part" Pad features.

SECTION 4
Other Notes on Publication

1. オプション設定 Option Settings
Go to Tools > Options > Part Infrastructure > General (tab) > External Reference (area)

"Only use published elements for external selection keeping link"
==> ON: Non-published elements cannot be selected.

"Publish a face, edge, axis, vertex or extremity"
==> ON: Can publish a face, edge, axis, vertex or extremity.
==> OFF: The elements above cannot be published.

2. パブリッシュ可能な要素 Elements below can be published
   -Point, line, curve, plane
   -Sketch
   -Body (Note: Geo Sets cannot be published)
   -PartDesign feature (CATIA settings)
   -GSD feature (e.g. Volume surface)
   -FSS feature
   -Parameter

土曜の朝は
猫が乗ってくる
二度寝もする

付記： 自分が沖縄でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。

AssemblyDesign (6) - Instance Names & BOM CATIA アセンブリデザイン基礎 (6)

製品構成番号と部品表 Instance Names & Bill of Material


「アメリカ人ですけど何か？」

*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


SECTION 1
製品構成番号の作成 Assigning Instance Numbers

1. Assigning Instance Numbers
1) Click on the "Generate Numbering" icon.
2) Select the top Product.
==> The "Generate Numbering" dialog box will be displayed.
3) Select a Mode option and click OK.
==> Instance number is assigned to each component.

2. Checking Instance Names
Right-click on a component to select Properties > Product (tab) > Instance (Number)
Using Instance Names
Create balloons in Drafting (Use the "Generate Balloons" icon)
Parts list


SECTION 2　
部品表の表示 Displaying Parts List

1. 部品表の表示 Displaying Parts List
1) In the tree, double-click on the assembly or sub-assembly to activate it.
2) Select "Bill of Material" from the Analysis pull down menu.
==> The "Bill of Material" definition box will be displayed.
3) In the definition box, click the "Define formats" button.
==> The "Bill of Material: Define formats" window will be displayed.
4) In the "Displayed properties" column of the "Properties for the Bill of Material" area,
select the items to show up on the list. Click OK when finished.
==> The changes will be made to the list in the "Bill of Material" window. Click OK to close.
(Note: The changes made to the above procedure will not be saved in CATIA. The settings will be
kicked back to default the next time you launch CATIA.)

2. 部品表のファイルとして保存 Saving the List as File Format
1) In the "Bill of Material" window, click on the "Save As" button.
2) Save the list with one of the available file formats.
Available formats: .txt (Note pad), .html (HTML), .xls (Excel)

3. 部品表をドラフティングに作成 Displaying BOM into Drafting
Created BOM can be displayed into Drafting.
(Additional Note: Material and mass can be added by accessing "Properties".)

4. リスト作成レポートの表示 Displaying a Listing Report
1) Activate an assembly or sub-assembly by double-clicking it in the tree.
2) Select "Bill of Material" from the Analysis pull down menu.
==> A dialog box appears.
3) Go to the "Listing Report" tab.
4) Specify the displaying items in the "Displayed properties" column.
5) Click on the "Refresh" button to create a list report. Click OK when finished.

5. リスト作成レポートをファイルとして保存 Saving a Listing Report as File Format
(Note: Only ".txt" format is available.)
Use "Save As" in the Bill of Material" definition box.

Photo taken at a Chinese buffet restaurant
Love the sushi here :))
中華の食べ放題で寿司ばかり喰う

付記：
自分が沖縄でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。

AssemblyDesign (5) - Enhanced Scenes CATIA アセンブリデザイン基礎 (5)

シーン(Enhanced Scenes)について

 

土曜の朝は 静かで良い

*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan
 
シーンについて　About Enhanced Scenes

SECTION 1 
シーンって何？　What is an "Enhanced Scene"?
"Enhanced Scene" is a functionality in an Assembly data that enables you to work on an alternative state of a product. This command allows you to explode assembled parts and keep both conditions (assembled and exploded conditions).


SECTION 2
シーンを作成　　Creating Enhanced Scenes
1. Click on the "Enhanced Scene" icon.
2. Select the "Automatic naming" check box.
3. Check "Overload Mode" and click OK.
==> The background will be displayed in green. This means you are now in the "Scene" mode.
4. In the Scene, change the parts location using commands such as "Explode".
5. When the work is finished, click on the "Exit Scene" icon to exit the Scene mode.
==> The background is now displayed your default color.
==> Makes sure the Scene information is created in the tree (named such as Scene.1, etc.)


SECTION 3
シーンを編集　　Editing Enhanced Scenes
1. Entering Scenes
(A) From the spec tree
Double-click on "Scene.xx"
==> You will enter the Scene to allow you to modify it.
(B) From Scene browser
Click on the "Scene Browser" icon.
Double-click on the Scene you would like to modify in the browser.
==> You will enter the Scene to allow you to modify it.

(*Note: This option is available only when "Activate an Enhanced Scene" is checked, which is accessible from the "Customize" button in the "Scene Browser" window.)

2. Deleting Scenes
Scenes can be deleted in the spec tree.


SECTION 4
1. シーン内での設定について  Settings for Enhanced Scenes
Available setting options for Scenes are the following. (Note: The information here will not be affected on the Assenbly data.)
- Location of components
- Show/Hide status of components
- Colors of components (Graphic properties)
- Activate/Deactivate status of components

2. 属性の修正   Modifying the Attributes
==> Modify the location of the parts and go back to the assembly. Make sure the assmebly is not affected by the scene.

3. 視点の修正   Modifying the View Point
Use the "Save Viewpoint" command. (Camera image icon)
==> Exit the scene and make sure the assmebly is not affected by the scene.

4. アセンブリへのシーン適用  Applying an Enhanced Scene to an Assembly

Use the "Apply Scene on Assembly" command.
==> The "Apply" window will be displayed. In the Product Selection list, the attributes that are changed will be indicated with "x". Select components you want to apply the attributes to the assembly data. In the right side column ("Attribute management" column), select attribute check boxes you want to apply to assembly. (Make sure the "x" mark will be changed to Applied.)
- Now, repeat this process on other components you want to apply the attribute changes into the assembly. - When finished, click on the OK button. Exit the Scene, and confirm the changes you
made to the assembly.

5. シーンへのアセンブリ適用   Applying an Assembly to an Enhanced Scene
Use the "Apply Assembly on Scene" command.


6. "多重定義モード"について  About "Overload Mode"
"Overload" is meant to be the situation where Assembly and Scene have different attribute information respectively.

Reference I
Two (2) oprtions for "Overload".
Partial: Overloaded partially. File size is smaller compared to the condition when "Full" is seleted.
Full: All attributes are overloaded.

Reference II
The "Overloaded Positions" icon can be used only when "Partial" is selected for the "Overload".


7. シーンを図面に落とす  Creating Drawing views from Enhanced Scenes
Exploded conditions of assembly data can be output into a Drawing.

目を閉じても 見られている

付記：
自分が沖縄でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。

AssemblyDesign (4) - Links in Assembly CATIA アセンブリデザイン基礎 (4)

Editing Parts within an Assembly Structure
アセンブリ内におけるパーツの編集

I need to go further ahead down this road. That's why I am here.
ここを通って もっと先に行かないといけないので ここを走っている

 

*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


SECTION 1

• リンクなし　Without links

1. 外部参照に関する設定  CATIA settings for external references
Go to Tools > Options > Infrastructure > Part Infrastructure > General (tab)
Remove the check for "Keep link with selected object".

2. リンクなしの新規パートを作成  Create a new Part without links
Scenario:
1. Create a new Part file under an Assembly.
2. In the Part file, create a box.
3. Insert another new Part file under the Assembly.
4. In the second Part file, create a lid of the box. Use the first Part's edge when creating a
sketch.

3. リンクがないことを確認  Confirm there are no links
Check the second Part file information in the tree. (Check the tree icons.)
Referenced elements from the first Part are displayed with red lightening marks in the tree.
Change the size of the box (first Part) and make sure the lid size will not follow this change.


SECTION 2 

• リンクあり　With links

1. 外部参照に関する設定  CATIA settings for external references
Go to Tools > Options > Infrastructure > Part Infrastructure > General (tab)
Check "Keep link with selected object".

2. リンクありの新規パートを作成  Create a new Part with links
Follow the same process as in the "Scenario:" described previously.

3. リンクがあることを確認  Confirm links have been made
Check the second Part file information in the tree. (Check the tree icons.)
Referenced elements from the first Part are displayed with green diamond marks in the tree.
Change the size of the box (first Part) and make sure the lid size will follow this change.


SECTION 3
アセンブリフィーチャー　Assembly Features
Assembly feature commands make it possible to perform operations to multiple Parts. The Assembly features include the Split, Hole, Pocket, Add, Remove, and Symmetry icon commands. There are icons with the same names in the PartDesign workbench, however they will be applied only to the features within the Part file you are currently working.

付記：
自分が沖縄でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。


話しかけたい 猫だから

［日記］ 昭和の詩人・西脇順三郎、そして連休初日（May 23, 2014）





the south wind has brought soft goddesses... it has wet the bronze, wet the fountain... swallow's wings... it has wet golden feathers... the tide water... the sand, the fishes... it has gently wet the temples, baths, and theaters... And this procession of gentle, soft goddesses has wet my tongue...

https://twitter.com/J_Nishiwaki_bot

The most significant point of the literature I believe is not the thoughts and ideas themselves, but the lights or reflections coming out of them. I think what makes literature valuable is not the gem, but the reflections it gives out.
 



words of surprise coming out of a woman... are reflections Cleopatra displays when she is praised... while pouring liquor...

Can't for the life of me recall how to spell the word "bara (rose)" ... every time i have to write it ... i look it up into the dictionary... what a shame... i stick out my sad head in the dawn... the window remains lonely...

それは昼どきだからです

 

自分はなぜだか、この西脇順三郎という昭和時代の詩人が好きで、一番最初に彼の詩を目に触れたのは高校生時代の日本語の教科書であったけれど、確かAmbarvaliaとかいうタイトルの詩集から抜粋した一節で、そのバタ臭さ満載な作風にいやらしさを感じつつも、自分は心のどこかに引っ掛かりを持ち続けていたのか、ある時点において、その引っ掛かりに導かれるかたちで『旅人かへらず』という、５７５に則（のっと）らない形式で表現した俳句のような、そのくせスカしたような物の書き方に好感を覚え、「無意識の心を書き記す」ということについて一つの新しい自覚の念が生まれたという意味において、あれから20年以上たっても気になり続ける存在なのだから、きっと自分はこの詩人の書くものが好きなのだ、と判った次第です。

彼はTwitter向けな作風の詩を書いていたんだな、と今思います。もしネットの時代に生きていたら、何を書かれていただろう？と空想することは心楽しいけれども、おそらくネット社会に害されて意外につまらない方向に変貌している可能性もあるのかも、などと意味のない思いを巡らせつつ、ともあれ本日は4連休の第1日、朝には娘を学校まで車で送り、その後は細君連れてNoviまで車を走らせ日本のカレーその他の食材を買ってくる予定。

ところで、娘と彼女の友達と昨日の夕方にドライブした際、彼女らが言うに、その日トヨタ自動車の社長さんが高校に訪問されたとのこと。

色を論じると　味を忘れる

Philadelphia roll my wife made
私はただ腹が減っている

 

 

AssemblyDesign (3) - Working on Assembly Components CATIA アセンブリデザイン基礎(3)

アセンブリ内における構成要素の操作
Working on Assembly Components

気を許せば　猫



*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


SECTION 1
構成要素の削除  Deleting Components

Right-click on the component to delete and select "Delete". Click "OK" in the "Delete" dialog box.

Note: The "Delete all children" option makes it possible to delete the assembly constraints that have been created with the component. (This option has been turned OFF by default.)


SECTION 2
構成要素のコピー、貼り付け  Copying/Pasting Components

Right-click on the component to copy, and select "Copy". Right-click on the assembly in the tree where you want to paste the component. Pasted component will be placed at the same location where the original exists. Whether the constrains will also be copied & pasted can be controlled by the CATIA settings. Go to Tools > Options > Mechanical Design > Assembly Design > Constraints (tab), and find the "Paste components" area that has the following options.

A) Without the assembly constraints
Assembly constraints will NOT be copied when the components are copied & pasted.

B) Without the assembly constraints after a Copy
Assembly constraints will be copied only when the components are copied & pasted.

C) Without the assembly constraints after a Cut
Assembly constraints will not be copied only when the components are cut & pasted.

D) Always with the assembly constraints
Assembly constraints will be copied when the components are cut & pasted, as well as when they are copied & pasted.


SECTION 3
「パターンの再利用」の機能を利用した構成要素のコピー  Copy Components With The "Re-use Pattern" Functionality

1) Click on the "Reuse Pattern" icon and check the "generated constraints" option.
2) Select the pattern you want to re-use from the specification tree, such as "Rectangular Pattern.1" or "Circular Pattern.1".
3) Select the component to copy, and click the OK button.


SECTION 4
構成要素の複数インスタンス化  Multi-instantiating Components

Components will be instantiated in the specified direction, with the specified spacing.

1) Click on the "Multi Instantiation" icon and select a component you want to multi-instantiate.
2) Enter the number of instances and the spacing (mm).
3) Define the reference element to indicate the direction of the instantiation, and click the OK button.

Note: The "Fast Multi Instantiation" command can be used when instantiating other components
with the same condition.


SECTION 5
対象による構成要素のコピー  Copying Components Symmetrically

Components (Parts or Products) can be created with the "Mirror" functions. Use the "Symmetry" command and define conditions in the "Assembly Symmetry Wizard" window.

Components (Parts or Products) can be created with the "Translate" functions. Use the "Symmetry" command and define conditions in the "Assembly Symmetry Wizard" window, but check the "Translation of new instance" option.


SECTION 6
構成要素の置き換え  Replacing Components

Components can be replaced with another component with the following process.

1) Right-click on the component to replace, and select Components > Replace Component.
2) The "File Selection" window will be opened. Select the component to replace with.
3) The "Impacts On Replace" window will be displayed. Make sure "Yes" is checked for "Do you
want to replace all the instances of the selected element?" shown in the window. Click OK, and the existing component will be replaced with the new component.

Check the constraints status in the tree. If the constraints are lost in the assembly data, a warning mark is displayed on the tree icon. User needs to re-define the constraints. Double-click on the constraints in the tree and reconnect the elements.


SECTION 7
構成要素および拘束のリオーダ  Reordering Components/Constraints

A) 構成要素をリオーダするには  Reordering Components
Select the "Graph tree Reordering" icon.

B) 拘束をリオーダするには  Reordering Constraints
Right-click on the constraint in the tree and select ***.object > Reorder constraints.

C) 拘束のグループ分け  Grouping Constraints
Constraints can be grouped using the "Group in new set" function. Multi-select the constraints
and right-click to select Selected object > Group in new set.


付記：
自分が沖縄(ここの出身というわけではないです)でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。

時々雲ゆきが怪しいと会話が弾む

AssemblyDesign (2) - Moving Components in an Assembly CATIA アセンブリデザイン基礎 (2)

AssemblyDesign (2) - Moving Components in an Assembly

ももちゃん ８：４９

*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


SECTION 1 
アセンブリ内で構成要素を移動するには  Moving Components in an Assembly

A) Using the Compass
1. Place the Compass on the component

2. Move the component using the Compass
Put the cursor on the linear portion of the Compass, and move the cursor in order to move the
component horizontally or vertically. Planar areas of the compass can be selected to move the component along the planar portion you manipulate. Arc portions of the Compass can be selected to turn the component. The top of the Compass (green dot) can be selected to move the component based on the origin point of the Compass.

3. Resetting the Compass
After finishing manipulating the components, the Compass needs to be placed back to where it was.
 a. From the menu bar, select View > Reset Compass.
 b. Hold the Compass directly in 3D, and drag it to the axis image shown on the right-bottom
area of the screen. 
 c. Drag the component to the 3D background with the "Shift" key selected.


SECTION 2
構成要素を数値を使って動かすには  Moving Components with Numerical Values

After placing the Compass on the component, right-click on the Compass to select "Edit".
A dialog box will be displayed. The values shown as the "Position" is where the Compass's
handle is located. Move the component numerically in the dialog box, by the axis direction,
angle, increments, or measures.


SECTION 3
アセンブリ・コマンドを使って構成要素を動かすには  Moving Components Using Assembly Icon Commands

A) Use the "Manipulation" icon
B) Use the "Explode" icon
C) Use the "Snap" icon


SECTION 4 
アセンブリ拘束の作成  Create Assembly Constraints

1. Apply the "Fix Component" command to the one that will be the base component.
2. Use the Compass to roughly place other components, so constraints can be performed easily.
3. Apply Assembly constraint icon commands (e.g. Coincident, Contact, etc.)
4. Update the Assembly data to reflect the constraints you have made to the geometries.

A) Option Settings To Manually Update The Assembly Constraints
Go to Tools > Options > Mechanical Design > General (tab). Check "Manual" in the "Update" area.

B) 3D領域に表示されるマークについて  Marks that will be displayed in 3D

Fix mark: Looks like an anchor. This mark indicates the component has been fixed with the "Fix Component" command.
Coincidence mark: Displayed with green circles, indicating the elements have been constrained
with the "Coincidence" command, by the axis, plane, or point.
Contact mark: Displayed with green square marks, indicating the elements have been constrained
with the "Contact" command, by the face or plane.
Offset mark: Displayed with linear arrow marks containing numerical values, indicating the
elements have been constrained with the "Offset Constraint" command.
Angle mark: Displayed with arched arrow marks containing numerical values, indicating the
elements have been constrained with the "Angle Constraint" command.

C) 作成した拘束に基づいて構成要素を動かすには  Moving Components Based On The Created Constraints

There are 2 options to move components based on the constraints you have created.
1. Move the component using the Compass while the "Shift" key is pressed.
2. Use the "Manipulation" command, with the "With respect to constraints" option checked.

D) 複数の拘束を一度に作成するには  Creating Multiple Constraints At A Time
1. Default mode: Used to create multiple constraints in a 1 versus 1 manner.
2. Stack mode: Used to create constraints between 1 element and multiple elements.
3. Chain mode: Used to create constraints such as between A and B, B and C, C and D, D and E (...)


E) アセンブリ内の構成要素を検証したい Studying Components in an Assembly

1. 測定  Measuring
2. 物理特性の確認  Confirming Physical Attributes
3. 最短距離の確認  Measuring Minimum Distances
4. 干渉の確認  Checking Clashes/Interferences
A) Use "Compute Clash" or "Clash".
B) "Compute Clash"
C) "Clash"
D) Export interference information into .txt file or .xml file.

Before exporting into a txt or xml, confirm the status by going to Tools > Options > Mechanical Design > Assembly Design > DMU Clash - Process (tab). Check "XML Export for  clash process　purpose".

F) 干渉結果の表示  Display of Results for Clashes/Interferences
List by Conflict (tab) & List by Product (tab)
Configured "Sag" values can affect the clash/contact results. Circle (cylinder) geometry is tessellated (approximated) in the program. The smaller the sag value is, the more closer the created circle is to the real circle.

G) サグ値の設定  Configuring The Sag Value
Sag values can be configured by accessing Tools > Options > ...


SECTION 5.
セクション作成  Sectioning

A) Select the "Sectioning" icon.
B) Defining the section plane
C) Use the "Positioning" tab in the Sectioning definition box.

"Normal constraint":  Move the section plane in the x, y, or z direction.
"Edit Position And Dimensions": Move the plane in the x, y, z direction by using numerical values.
"Geometrical Target": Select a face or edge of geometry to create a section plane that is
parallel to the selected element (face or edge).
"Invert Normal": The direction of the normal line to the plane will be inverted.
"Reset Position": Used to get back to the default condition.


ボリューム断面の作成 Creating a Volume Cut 
Section can be created in the geometry area. Inside of the cut geometry can also be viewed.

住宅地はTVよりも情報量が多い

付記：
自分が沖縄でCATIA講習を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。

AssemblyDesign (1) - Assembly & Components CATIA アセンブリデザイン基礎 (1)

アセンブリと構成要素  Assembly & Component

自分がCATIAの講習を初めて受けたのは日本の沖縄の土地においてで、そこに3か月ほど一人で滞在し、CADとかITとかが初めての経験だったこともあり苦労は大きかったし、途中で脱落しかけたけれども、今となってはとても大切な思い出として記憶しており、そういえば休日などは、食堂にトコトコと出歩きタコライスをよく食べたものだったことを思い出すにつけ、自分が憶えている沖縄のおいしい食事は沖縄そばでも何でもない、タコライスだった、と言うことができるほど好きな食べ物であったし、また休日といえば、一人で海辺まで出かけて行ったりしたことも忘れられない思い出として心に残っており、道中、ハブが出てきて噛まれはしまいかとドキドキしながら雑草生い茂る坂を早足で歩いたり、急な雨に降られたりもしながらも、バスを乗り継ぎながら目的地に行き、海岸をとぼとぼ歩き、暖かい風を感じながらゆっくり時間を過ごし、しばしそこの風景を楽しむと、またバスを乗り継ぎながら滞在していたレオパレスの部屋まで帰って行ったのだったけれども、なぜだかバス停で立って待っていてもバスが何台も通り過ぎてしまい、あれはなぜだったのだろう、バス停ではないものをバス停と思い込んでいたのだろうか、などと思ったりした次第です。

沖縄でのCATIA職業訓練コースののち、自分は千葉県と群馬県で仕事をすることになったのだけれども、毎日ノートPCをバックパックに担いで朝から就寝前までCATIAをやっていたことはとてもいい思い出で、群馬県のホテルに滞在しながらお客さんのところに通いヒアリング活動したり、CATIA教育をさせていただいたり、ワークショップ等でモデリング指導をしたり、プレゼンをやったり、仏ダッソーの開発元との電話会議をやったり、手順書その他のドキュメントを日本語と英語の両方で書いたり、ずいぶんいろんな経験をさせていただき、その期間中、当時リーダーだった方からは多くのことを教えていただいたり、また面倒も見ていただいたことは、今思い出してみても楽しいもので、焦ったり、ストレス抱えて仕事をしていた部分もあったに違いないし、家庭を持つ身でありながら月給が手取りで12万円程度で、周囲を心配させるほど生活が厳しかったのだけれども、良い思い出ばかりの、実り多い時期だった、と感じ入っているのが本当のところです。


*沖縄のCATIA職業訓練コースで自分が取っていた覚え書きから
*From my memo I was taking during my CATIA job training course in the Okinawa island, Japan


Assembly (アセンブリ): Also known as a "Product". This is meant to be a collection of multiple Part
files.

Component (構成要素): Parts that build up an Assembly.
Part: Data created in the PartDesign or Generative Shape Design workbench.
The top Product file can contain either Part or Sub-assembly data. Sub-assembly data contains
its own components (Parts/Sub-assembly) inside.


パーツ名とインスタンス名  Part Numbers & Instance Names

Part number (パーツ名):  The name of a component. Every Part or Assembly has its own Part number.

Instance name (インスタンス名): The component name that will work as the identifier. When the same component (of the same Part number) is inserted into the Assembly data, different instance name will be assigned so the system will not mix them up.


パーツ名とインスタンス名の編集  Editing Part Numbers & Instance Names
Part numbers and instance names, by the way, can be modified from each "Properties" (or just
hit "Alt+Enter" on the component name in the tree). In the specification tree of Assembly data, user needs to be aware which component is in active state. Even when you are working in an Assembly, if a Part file is activated, the current workbench will not be the Assembly Design workbench, therefore you will not be able to see Assembly Design commands (icons). Also, if you want to modify a specific Part and the top Product is activated, the Part Design/Generative Shape Design commands are not available. (Modification cannot be performed with that condition.)


活動化状と態選択状態  Active Status & Selected Status
Active status (活動化状態): Active status means you are currently working in that component. In the tree the active place is colored with a blue background. Double-click on anywhere you want to activate in the tree.

Selected status (選択状態): Selected status means you have clicked on that component most recently. In the tree the selected (single-clicked) place is colored with an orange background.


パートデータとプロダクト(アセンブリ)データ  Part Data & Product (Assembly) Data
One of the biggest differences between Part data and Product (Assembly) data is whether
clashes/interferences can be checked or not. This indicates that if the whole data is created in Part,
each components will not be as flexible as the Assembly data with the same geometries. Assembly
Design workbench has various constraint command icons, whereas PartDesign or GSD doesn't.


構成要素の挿入  Inserting Components
Select the "Existing Component" icon. In the tree, select the Assembly you want to insert the component. In the browser window that is opened automatically, select the inserting file, and click on the "Open" button. Selected component will be inserted into the designated Assembly.

Another way to do the same thing is to right-click on the Assembly you want to add a component
into, and select Components > Existing Component.


新規構成要素の挿入の際は
When inserting a new component, a message box appears to ask you if you want to specify the
origin point. If "Yes" is clicked and select a specific point, the component will be inserted so the selected point will be defined as the origin point. If "No" is clicked, the component will be inserted so its origin point will be the same as the top Product's (top Assembly's) origin point.

There is an option setting to display a pop up box so a Part number can be entered when adding
a new Part.
Tools/Options/Infrastructure/Product Structure/Product Structure (tab)


カタログからの挿入も可  Inserting from the Catalog
In CATIA, components can be inserted from the "Catalog Browser" command.


アセンブリデータの保存  Saving Assembly Data
We use "Save" or "Save As" when working in MS Word, Excel or PowerPoint. There is other save command that is often used in CATIA but doesn't exist in other applications such as MS Office
products. It is "Save Management".


なぜ「保存管理」なのか  Why "Save Management"?
Save Management needs to be used when working with an Assembly data or CAE data because the
data contains multiple Part files (or Product files) and they all have to be taken care of, including each one of its file name and save directory. When user wants to change a file name in an Assembly, working in the Internet Explorer will not be good. This is because, by changing a file name in the Explorer window, CATIA will miss out the information on the modified file. (Let CATIA take care of the file information. Do not use Windows Explorer when modifying the file names.) Also, the save location is also important to be recognized in CATIA, since not all components (Part files, Product files) are saved in the same folder location on the system or network. If you have a component named "MyScrew1.CATPart" in some network place and have used it in an Assembly, but you already have modified version or back up version with the same file name in different places. Which one does CATIA refer to? - Save Management is a useful tool in order to avoid such a conflict.

付記：
自分がCATIAの研修を受けた際にとっていたノートを元に、おおまかな知識を書き出してみたのだけれども、久しぶりに見直してみて、随分いろんなことを習ったものだと改めて思うに到り、中には今になって、なるほどそういうことだったか、と合点のいくものもあったりで、復習をしてみる意味においても、当時のメモやノートを掘り起こすのは悪くないかと思い、書いてみた次第です。