Boolean Operations In CATIA V5.

Hi all

It is a long time I did not wrote anything. I was bit busy with my personal work.

Let’s start with Boolean operations; many people don’t know how to use these 6 commands (Assemble, Add, Remove, Intersect, Union trim and Remove lump).

What is Boolean operation?
-->Boolean is an operation we can Unite two different bodies together or subtract one from another.

In Catia you can insert "N" number of Bodies, Body2, body3, body4,........so on.
You can insert new body by pull down menu INSERT---------> Body.
Under part body create a 100mm X 100mm sketch on XY plane and extrude it by 25mm.
Now insert another body that's body2, now create a sketch on YZ plane 50mm X 50mm and extrude using pad command around 50mm, make it mirror Extend. This block should penetrate the block which created under part body.
IMP Note: you might have observed the " + and -" symbol on body2 or body3. It’s called Polarity of that body. The Polarity of the body will be decided by the first feature used in that body. Ex: Instead of Pad if you use a pocket the Polarity will be negative, all positive feature henceforth became -ve like PAD, SHAFT, RIB...., and _ve features became positive like POCKET, GROVE, SLOT.....

Now insert another body i.e. body3 and create sketch on ZX plane, extrude using pocket it has to intersect/penetrate through both the blocks. Now Body3 having –ve Polarity”

1 Assemble.
The assemble command work on depending on the polarity of the bodies. Now select Assemble command then select Body2 (If you select Part Body you will get error) pop-up will appear, in that you can select part body, then you click on preview then Ok. Here now it will remove only Intersected material between two selected bodies. If you select body3 which is having _ve polarity, then you select either part body or body2 it will remove now, whole body3 and where this body is intersected with the selected body. If you select body2 then body3 here it will remove body2 and where this body is intersected with body3.
It’s clear that, if you select two bodies which are having same polarity It will remove only Intersected material between two bodies. If you selecting two bodies which having both +ve and –ve polarity, in this case it will remove the first selected body and where it is intersected with 2nd body.
2. Add
In add option irrespective of polarity of the bodies it will remove only intersected material between two bodies. Here the bodies may be +ve or _ve or any combination.
3. Remove
In this feature also it never bothers whether the bodies are +ve /-ve or the combination of any. It will remove first selected body and where it is intersected with the second body.
4. Intersect
To get a common material between two bodies we can use this option. Here also it won’t bother whether the bodies having different polarities.
5. Union Trim
Using this option we can remove unwanted material from both the bodies. We can use this option to create T joint for pipes.
6. Remove lump
This option is used within a body to remove unwanted lump in the body. Here we can use this option even in part body also. Assume you have “N” number of lumps in those if you don’t need some of the lumps you can select the face of the lumps which you don’t need then you can say ok it will remove all the lumps which faces you have selected. If you select both faces to remove and faces to keep and if you leave some lumps In this case it will remove the lumps which you have not selected. When you using this command I suggest please select only faces to remove or faces to keep, that is enough.
Interview questions on Boolean operations:
1. What is the difference between assemble and add.
2. What is alternative option for intersect in part design.
3. What is alternative option for remove lump in part design?
4. What is polarity of the body?
5. Is it possible to change the polarity of the body?

Sketcher

We can enter in to Sketcher. To enter sketcher work bench follow these steps.
1. Open Catia V5
2. Close the module which has opened ( Default it will open Product structure)
To close this module, go to FILE pull down menu, click on close, it will close the module which has opened.
3. Now again go to START---- Mechanical Design---- click on Part Design Instead of Sketcher.
4. Pop-up will open, please enter part name else default will be Part1. Uncheck Enable Hybrid Design ( I will Explain what is Hybrid design later) then click OK.
5. Now you entered in to Part design.
6. Create Axis system.
Go to INSERT ---- Axis System, click here .In the popup it will ask origin, Right click on no selection, click on Coordinates, enter the values as (x=0, y=0, z=0) because I don’t know where the part will be placed in an assembly, later you can change the coordinates.
7. Select all principle planes by selecting from specification tree, (XY, YZ and ZX planes just below the Part name) then right click, select Hide/Show. It will hide these planes.
8. Now select a plane from Axis system (say YZ plane) then go to Insert pull down- Sketcher, click on Sketcher option. There is positioned sketch we can see that later.
9. Now you are in Sketcher work bench.
The important Tool bars in sketcher are
a. Profile
b. Operations
c. Constraints
d. Sketch tools
e. Visualization
f. Knowledge
g. Tools
h. Work bench
Before proceeding we can see the mouse operations and some shortcut keys
Mouse operations
1. Left mouse button-- Select
2. Middle button / Scroll ------ for Pan a component. If you rotate scroll specification tree will move Up and Down.
3. Right mouse button: it work with combination of middle button.
4. Middle button+ right/Left----- For Rotate
5. Middle button+ right/Left once click and release----- For Zoom in Zoom out
In your mind these questions may arise.
1. Why it’s not possible to enter Sketcher workbench directly?
2. Is it necessary to disable hybrid design?
3. What is model tree/Design Tree/ Specification Tree?
4. Is it necessary to create axis system?

Axis System in Catia V5

Let us start with Axis system
The basic question when you starting any new part/Component.
why local Axis system is necessary even if you have a global axis?
Is it necessary to create Axis system?
Yes ! you must create Axis system when you starting new part.

Assume you are creating a parts for a Automotive or Aerospace or any heavy machine tool. The assembly is having thousands of components in it.
If you use a global axis system to build/Model all the parts.
1. Its very difficult to assemble in assembly, when you import these components to assembly.
2. When you import all parts, all parts will come and sit on global axis system in assembly
3. You need to separate/ move all the parts apart.
4. you need to Identify where the components will be fit in assembly.

To avoid all these errors you need to create axis system when you starting new part.
Assume you are creating a rare wheel of a car. first thing you should know where and at what distance from global axis in car it will be fitted.Take the Coordinate(X, Y, Z)Using these Coordinate values you fix axis system and create a wheel. when you import this part in Car assembly it will sit at its position. No need to give a constrain again.

I will give one more Example. assume you are creating table and your laptop or Monitor placed on it at a center of the table top. ( Assume here table is a single part and your Monitor also single part)Just I want to create assembly of these 2 parts.
1. Take lower left corner leg of table as Global origin. model the whole table as a single part.
2. Measer the co-ordinates(XYZ) for center point of a table top.
3. When you start creating new part say Monitor, Using those value of XYZ what you got from table part create a point using Coordinate method 3D point then place a axis system on it.
4 make the monitor base center point as symmetric about the axis, then create whole monitor
5. save these two files separately
6. Import these 2 parts to assembly, automatically monitor will be placed on your table top.

How to create this axis System in part design by two ways.
1. Go to pull down menu -->INSERT------> Axis system
2. Select a command Axis system from Tools tool bar.

It will ask you the origin in pop-up menu, you just right click and take an option Coordinate. enter the values for X, Y and Z. then click OK.
Local axis is placed now at required location. Some time you you don't know the axis system location just enter 0, 0, 0 . later when you get the co ordinate values you just edit the values the part will be moved to that location along with your axis system.

CATIA a Master Tool for Design.

Dear friends
As I know Catia is a more powerful and user friendly software in CAD. You can create complicated models very easily in this software. I was a teacher for Catia for few years. I know little bit about this software. I am not an expert According to me, for few of them I am a master. I trained more than 2000 professionals on Catia. I never gave notes for my students because I hate writing notes in class. Most of my students are working in all over the world in Various Companies in Aviation and Automotive field. Some people are working as corporate trainers in India. I never had undergone any corporate training. Here I am going to write about CATIA V5 tips and how Commands work in some of the workbenches. It may help you when you stuck up. I concentrate on
1. Sketcher
2. Part Design
3. Generative Sheet metal
4. GSD
5. Drafting
6. Assembly
7. DMU Kinematics.
I always welcome your Suggestions....