Coordinate Dimensioning CATIA V5

[Acee]

Hi,

If I have a part designed in CATIA V5 in body position away from the origin but on the drawing I want one corner of that part to be 0,0,0 and have everything measured off of that corner how is this possible without moving the part? I have created an axis and made it current but this does not seem to effect the drawing or the 3D measurement unless you toggle the other axis option in the measurement tool but this is only temporary. In V4 when we create a new axis and make it the working axis that point becomes 0,0,0 in the model and drawing why does this not work in V5? I appreciate any input into this topic. Thanks,

 

[Azrael]

What kind of measurement are talking about? Grid? Hole positions? If creating a hole table then u can chose which axis to use. But if it's the grid I'm not sure how to do it easy, at our company we use a macro.

 

[Acee]

It is actually for another group at my company but what he wanted to do was use the 3D coordinate call out for tube bending. I told him he could use a coordinate table but even with that option I am not sure if you can select a different origin point. He wanted to use a selected 0,0,0 as a datum and then measure each bend point off of that specified point but the point he wants is not the origin of the model. I do all my work in body position so I have never run into this issue. I was trying to help a co-worker so any information will be useful. Thanks,

 

[Albigger]

You can actually pick any reference in your drawing to use as 0,0 when using the cumulated dimensions.


If you actually want the blue H and V lines in that position, then you have a little more work to do. Create an axis system at the desired origin in the 3D model file. Then when you bring in a view, pick that axis system (in the tree) BEFORE picking the view plane.

That should do it.
--Jay

 

[Azrael]

You can select a different reference axis with point table. But for coordinate callouts it won't work, then I would go with Albiggers suggestion

 

[Solidkat]

This might work for you:-
Place a point in the model where you want 0,0,0 to be and then in the drawing turn on 3d points in properties/view and take all your dimensions from that point.

 

[Acee]

Thanks for all the suggestions. I tried Albigger's suggestion and this seems to work for the coordinate call outs and I believe this is what the guy is looking to do. I will show him these suggetions and I think he will be able to do what he wants. Thanks again.

 

[Acee]

Ok so here is the deal with this. If I use this method in a CATPart it works great when I select the axis before creating the view it becomes 0,0,0 in the view and everthing is measured from that origin.

However, when I do this in an assembly that point becomes 0,0,0 on the part where the axis is created and every other component is measured off of that origin only where it was created but not where it is positioned in the assembly. So if I have an instance of a component 8 times in the assembly in 8 different positions each time I add a 3D coordinate callout it is the same coordinate in all positions??? This is strange because if I create a view without changing the origin all the instances have different coordinate locations. It seems that when I change the origin before creating the view it only measures each instance from where it exists in the component and not the assembly. Has anyone run into this problem?? Does anyone actually understand this problem??