2 tubes

[klaas2]

i really have a problem in catia5 r14 to make a assembly of 2 tubes together
1 want to make a setup where i can make a variation in tube lenght
and the tube ends must merge to gather
you must see that as a bike frame
so differant in height and angle's
i cannot get it done
i also cannot use the tubing option since all tubes are not the same
seat tube is differant the head tubes and so on also the are not also round but a certain defined profile
i try simple to connect 2 tubes under a angle let say 72 degrees and try to seamless merge them together but the ends have to be defined before them putting together and that i cannot know the end how that profile looks like
that is why catia has to do for me
am it on the wrong way or cannot be done !
help!!!!!!!!!!

 

[jackk]

Klass...

If I understand you correctly, here's what I would do:

1. use the Part Design workbench for the tubes - not Tubing
2. I'd setup some parameters to control the length of the tubes, the angles, etc.
2. make a sketch of the tube profile (OD and ID profiles) and use a pad (or rib) to make the tube
3. make each tube in a separate CATPart, with all the parts in a CATProduct
4. here's how I would do the end cuts: (lots of other ways)
Tube 'B' is cut to be welded onto Tube 'A'
a. copy and paste special with link the partbody of 'A' into the 'B' part
b. in the 'B' part insert a boolean operation to remove 'A' from 'B'

 

[klaas2]

yes i uderstand what you say i try to do this but i could not succeed in doing so

it s trange question but is it possible you sent a jpg of the 2 tubes and the tree so i can see how you did it
i find a strange thing that i cannot get it done
assume 1 tube is at a angle of 72 degrees to the other

can you do that i would be very grateful
klaas

 

[jackk]

here's a quick version that shows parameters and the boolean remove:

 

[catiajim]

I'm not sure what the problem is here. It looks to me like you successfully trimmed the end of the blue tube. Are you trying to put a hole in the yellow tube as well? If this is the case, you will need to have some kind of intermediate part here, as you cannot have the Yellow tube linked to the Blue Tube which is linked to the Yellow tube.

Youre best bet would be to create a Control Part (sometimes called a Skeleton Part) that consists of nothing but the centerlines of all of the tubes. You would then link each of the Tube Parts to the Control Part. That way each part is only linked to the control part, not to each other.

I would also make sure that all of the lines in your Control Part are Published. This action puts a special identifier on the element that will greatly ease your ability to maintain and change your links.

 

[jackk]

Klass...

Jim is correct about using a "skeleton part" containing master geometry and parameters.

But Jim's method is an advanced lesson. In my 'quick' version, my intent was to keep things simple and only show you PARAMETERS and the BOOLEAN REMOVE. I think these are what you were looking for in your original post.

...Jack

PS: sorry for the big image - I should have cropped it!

 

[klaas2]

yes i think i need the thing catiajim suggest
all tube are hollow and with holes fixed to each other

can ask you jim in wich work bench you woul do this and how you proceed meaby a example because i never did what your suggest
it sounds for me the solution
so i can have each line linked to its tube style and length
this is waht you need with a bike frame not all round tubes and i want a seamless connection for later analyses of the fittings like carbon tubes to lets say titan tubes in all its variations
its stupid just can not find the right start
so can you me please to get this thing started
klaas

ps its possible with a screen dump from the work bench you are doing this in

 

[catiajim]

As jackk stated, this is an advanced lesson, but let me try to give a simple example.

The workbenches to use are Assembly Design and Part Design. In TOOLS --> OPTIONS --> INFRASTRUCTURE --> PART INFRASTRUCTURE, turn on the following options:
Keep Link with Selected Object
Only use published elements for external selection keeping link
Confirm when creating a Linkwith selected object (this one is optional, but I like to have it on to remind me that I am linking)

First, create your skeleton part. This part contains the simplified geometry of the entire bike. It is just lines and points, with some parameters for various angles and lengths. There are no solids in this part. For each of the centerlines, use TOOLS, PUBLISH to add a publication identifier to these elements. (Note: search the forum for more information on Publications).

Second, create a new Assembly. Add your Skeleton part to that assembly. Add a new part for the first tube, and make it active. Create your sketch for the tube, selecting the appropriate line in the skeleton. For the notches and holes, create more sketches and link them to the appropriate lines in the skeleton. Repeat for the rest of your tubes.

Note: You will not be linking to the solids in the other parts - only link to the skeleton. If you want to get real fancy, you could put the appropriate sketch for each tube shape into the skeleton as well (and remember to publish them). That way all of your tube shapes would be linked to the skeleton as well. Whenever you need to change the assemly, you simply make your changes to the skeleton, and update your parts appropriately.

For more information, please search the forums for Contextual Links. They are very powerful, but there are some things to watch out for. Somewhere there is an old whitepaper from IBM that talks about Links in general. There are also some very good articles in the CATIA Solutions Webzine (

http://www.catiasolutions.com)