Orientation of components in V5 2

What do you mean by "I need to file all the components in correct axis position individually so could not use product to do this."?

If you mean the individual detail parts must be "located" in their "correct axis" coordinates, good luck. You get to re-build each of them.

The best/fastest way to get all of the the parts in their "correct axis" position is to use Assembly Design, and constrain them appropriately. Alternately, you can use the Snap function (or if you have a DMU license you can use Cumulative Snap).

If you simply need a copy of this assembly all positioned properly, you can use the TOOLS, CREATE CATPART FROM PRODUCT after you have used Assembly Design to position everthing. This will merge all of the parts together into a single CATPart document, with everything in it's "Correct Axis" position.

Just remember, "Correct Axis Position" is all relative to the assembly. A bolt has a "proper position" in one assembly, and a different "proper position" in a different assembly (or possibly even in the same assembly). In a PLM environment, the "Correct Axis Position" of a part can even vary with time, effectivity, or serial number.

Catiajim,

I am an ex V4 user so might be using teh old school terms for some of the comments, I am have all the components at origin and am looking to relocate the parts to their correct orientation in car, it has originally been done by a data backbone and the files have been forwarded to us with out any axis orientation.

In V4 I would have oriented the parts with move and would have shifted between 2 axis. I would assume that there is a similar methodology in V5, this would then allow me to import a locator, hole centre / vector, and use this to orient the part in the part file. I will never have to modify the component so am not bothered about the geometry not being local if this helps.

You can use the translation and the rotation tools to locate the part in the "proper" position. However, it is quite time consuming to get the proper orientation of the part as you have to specify an axis of rotation and a rotation angle. I haven't found anything to orient a part along a specific vector (other than specifying a rotation about an axis). The best way to have the part in the proper position is to remodel the part in the proper orientation/position, as catiajim indicated.

Catiajim, what release of V5 do you have? I don't have the option to create a CatPart from a Product. It would be very useful when converting V5 files back to V4 format.

The truely best way is to use the Assembly Design workbench and create a Product. There you have a full suite of tools to move and orient the parts.

Create CATPart from Product is available GA at R14 (or so they tell me). It is available in R12 or R13 by setting the environment variable IRD_PRODUCTTOPART = 1.

Thanks Catiajim!

I agree that the best way is to use the Assembly Design workbench to position and orient the parts.

The only problem is when customers demand to have the parts located in "body co-ordinates".

Gents,

Thansk very much for all your input, I have discovered a solution which worked very well for me in this particular case. Most of the orientation had bolt holes and planar faces to locate on, as a result I have created, in a V4 fashion, local axes created on bolt hole centres and using teh planar faces to orient, I copied in the locating face data from the adjacent part and followed the same process. This then allowed me to use axis - axis translation to re-orient the component in it's own part file, a few quick isolates and I was left with just the axes which I slid into no show.

This explanation does not cover of course teh faffing around I did orienting the axes, surprisingly easy to muck up when you remove all reference data. But all done now, so thanks again for all posted assistance.

if u dont need the history of the part, what you can do is to place it in the assembly with the assembly tools.

then you have to create new empty parts inside the assembly using the same coordinate system than the assembly.Then you go to the part that contains the body or surface you need, you copy it, then go to the new part that has the same CS than the assembly and paste as result .

hope it helps