# couple of questions about Catia

I need some clarification about Catia
1. what is geometric set actual why we use and what about benefits of that.
2. what is different b/t geometric sets and order geometric sets.
3. how can I measure draft angle in surface and part.
4. what is hybrid system when we have to use it.
5. what is different b/t position sketch and normal sketch
6. and different b/t add and assemble boolean operation .

the main difference between the position sketch and normal sketch.....
in position sketch we can adjust the postiton of HORIZONTAL and VERTICAL direction before entering to 2d sketcher work Bench.. But in normal sketch we can enter into 2d workbench by default

assemble can be donebased on nature of the body(polarity symbol) but add is irrespective to the nature of the body it may be positive/negative body

by using the measure between we can find the draft angle

1)Geometric set is a 2D element in catia.. whatever the lines,points & sketches will come under geometrical set
2)For multiple operation(multiple bodies) we can use geometrical sets but ordered geometrical sets is suitable for single body in shape design
3)You can measure draft angle bu using the tool "measure between" ..it's icon looks like a vernier caliper
4)Hybrid system is used to interact between both surface and part modelling (In short hybrid is combination of both surface and part modelling)
5)Using position sketch we can draw sketch in all the 4 quadrants but in normal sketch it 'll take only one quadrant.
6)Assemble boolean operation will only suitable for positive operation but add option can be used in negative as well as positive operation.

Hello Ajay,
1. what is geometric set actual why we use and what about benefits of that.
I would say a geometrical set is a place where you will group sketches, lines, points and surfaces. You usually use more geometrical set to order your part into small groups so that it will me much easier to modify it later on.
The order of the operations is not important, you can group the operations as you want.

2. what is different b/t geometric sets and order geometric sets.
I never used it, but I know it is similar to a Body, in which the order of the operations are important and dependent on one another.

3. how can I measure draft angle in surface and part.
Manual mode: Use the measuring tool "measure between"
Automatic mode: Use "Draft analysis" tool

4. what is hybrid system when we have to use it.
Hybrid design is used when you want to have surface design and solid design in the same bodies. By not using Hybrid design you will have solid operations ordered in Bodies and Surface and Wireframe operations ordered in Geometrical Sets.

I do not recommend using Hybrid design, this is what makes CATIA special from other CAD software.

5. what is different b/t position sketch and normal sketch
In a normal sketch, the sketch is positioned automatically by the Global axis system.
In a positioned sketch you can position the sketch however you find it best for it's application, meaning you can control the V and H.

6. and different b/t add and assemble boolean operation .
First of all you need to know that you can have positive and negative bodies depending on how it was created (You can see the sign of the body in the upper right corner of the body icon)
The difference between ADD and ASSEMBLE operation is that ADD doesn't take account if the body is positive or negative.

For examble:
Add negative body2 to positive body1 = positive body1+2
Assemble negative body2 to positive body1 = positive body 1-2

Add positive body2 to positive body1 = positive body1+2
Assemble postive body2 to positive body1 = positive body 1+2

Add negative body2 to negative body1 = negative body1+2
Assemble negative body2 to negative body1 = negative body 1+2

Add positive body2 to negative body1 = negative body1+2
Assemble postive body2 to negative body1 = negative body 1-2

The best way to understand them is to do some tests. Try the combinations above and you will understand them for sure.