Some exemples of Inventor from Youtube

[Faouweb]

Hi,

I was looking for some Inventor's tutorials, and i have found some exemples:?

http://www.youtube.com/watch?v=zCgv4LYiIJ4&feature=related

for the last one how can i model the tyres?

[shift1313]

if i remember right that rc car model is in the inventor files.

 

The tire can be drawn with a revolved feature. The tread can be done using Offset surfaces and extruding a 2d sketch To/From using your surfaces. Then a circular array. Do you want to draw that exact tire or just a tire in general?

[Faouweb]

i have tried to draw the tyre, but it's difficulte to imagine the section's shape. where can i find a tutorial about that? Thank you.

[shift1313]

well the profile of each tire will be a little different but they will all have a 'bead' area where it matches the rim. here is a good cutaway of an old car tire.

 

 

here are some motorcycle cut aways.

 

 

If you are actually talking about RC car tires they are a little different because they have foam cores typically.

 

 

I will draw up a tire similar to the rc car tire and put up some screen shots for you.

[shift1313]

Alright here are some screen shots. Im not going to go into detail about each step because I am assuming you know how to properly sketch, setup sketch planes and dimension your sketches. If you have any specific questions about the procedure just ask. The profile was sketched, then revolved. An offset surface was created using Thicken/offset down into the tire(this is the "to" plane for the extrude/cuts and is highlighted by the dashed red lines in the 3rd pic). I created an offset plane to do my tire tread sketches. Firs was the zig-zag. I did an extrude-cut 'to' my offset surface. Circular array 5 times. Then i did another sketch on my offset plane projecting edges of two of the arrays and connecting them with lines. Extrude-cut, then array that 5 times and you should have a zig-zag around the tire. Next was the straight line all the way around the tire. I did this with a profile sketch projecting my offset surface and creating the rest of the profile. Then i revolve-cut this. Last was the "swoop" part of the cut away. Again extrude-cut this to my offset surface then a circular array(30 times in this case).

 

One important thing to note with extrude-cutting to your offset surface. This surface goes around the entire tire. You will need to use the "more" tab on the extrude pop up window and select "minimum solution". If you dont the cut will go through the tire and to the offset surface on the other side.

 

Hopefully the screen shots give you a little insight into one method of drawing the tire. Of course i could do this other ways by projecting paths onto my offset surface and doing sweep-cuts or any other number of ways im sure. The benefit of the sweep cut is being able to round the corners slightly without having to fillet. Not a huge procedure when using rule fillet but could be a time saver depending on the design intent.

 

 

 

 

 

 

 

 

 

 

[Faouweb]

Thank you very much i will try to do it :wink:

[shift1313]

also, someone on another board asked me how to draw a certain MC rim. It was a CNCd Marcheshini rim. I did the same thing with a bunch of screen shots during the progress. Its not how i typically draw rims but these are cut from a cnc blank all one piece so thats how i modeled it.

 

screen shots are in my photobucket.

 

http://s268.photobucket.com/albums/jj39/shift1313/cad/