The ordinate command is giving me grief

[CADWHORE]

Does anyone use ordinate dimensioning? It seems very clumsy and difficult to make it do what I want. I have a part that from the top view has radiuses on all 4 corners. I would like to make the intersection of the X and Y sides my ordinate basepoint. I can figure out no way to make it so. Even once I get this it is very cumbersome to pick anything but a hole. For instance the edge of a pocket or the outer edge of the part. It gives me two dimensions for everything I pick, where sometime only one is required. Do I just have to go back and delete the unwanted dimensions? Let me know if you have found a good way to make this function work for you. I am on NX4,

Thanks,

 

[JohnRBaker]

OK, when you select the Ordinate Dimension option and the Que line asks you to "Define new ordinate origin..." look for the 'Snap Point' toolbar and find the 'Two Pick Intersecion' option (should be the 2nd icon from the right-side). Select it and then you will be able to select the 2 straight sides of the model to define the virtual intersection as your Ordinate Basepoint.

As for creating only dimensions along one baseline and not the other, what you do after you've created your first dimension to define your auto-margins (or created explict margins), place your cursor over the 'baseline' axis that you wish to be ignored and press MB3 (right mouse-button) and select the 'Set Baseline Inactive' option. Now when creating dimensions the only ones created will be with respect to the OTHER baseline. To activate the baseline again or to switch which baseline is to be inactive, just repeat the above baseline selection procedure, picking the appropriate options.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[CADWHORE]

John, I wish you sat in the next cubicile over!! Thanks for your help on this, my company has provided no training on this software so it is very nice to get some answers from those who know.

 

[BOPdesigner]

I frequently struggle with the ordinate dimensions also and have wondered how to do that single baseline dimensioning also. Is there a way to have the ordinate dimension values aligned with the leaders, while maintaining horizontal alignment for the values of regular dimensions? After placing my ordinate dimensions, I have been picking the horizontal dimensions, going into the style dialog, and setting them to aligned each time.

 

[JohnRBaker]

Could you provide a pciture of what it is you're tyring to accomplish as I'm not sure exactly what it is that you're doing?


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[latchescmk]

BOPdesigner:
This is an option in NX5. I have long struggled with that same scenario. In NX5 you can set the ordinate to be "ALIGNED" while conventional dimensions can be "horizontal".

 

[rep001]

Another way is to use the utility symbol/ intersection, to make a point where the two edges would meet/cross. then, you can use that point and the origin.

 

[CADWHORE]

Thank you for the help on this problem. My next question regarding it is, how do I shoe the origin of the ordinate system? It only says "ordinate" with no reference to what I selected for the two baselines, which would make it very hard for the shop to build the parts.

Thanks

 

[JohnRBaker]

Where I came from, you always added a set of dimensions that referenced the two baselines so that you had a pair of 0.00 dimensions that indicated what the other dimensions were being measuring from.



John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/