I would like to know how to generate more results of values from NX 9.0 to MS Excel spreadsheet.
1) Now I interface model with spreadsheet so i can put a value (length parametr) to spreadsheet and update a model - it works - model changes size, but i would like to have a value of volume of current size in spreadsheet. I dont know if its possible.
2) I need this for lots of sizes (f.e.: 300 and more). It probably take a time.
Would anybody know how to solve this?
Solved! Go to Solution.
Menu > Analysis > Measure Bodies. Check the 'Associative' option under Associative Measure and Checking. It will generate the expressions for the Surface Area,Volume etc.
Tools > Spreadsheet, In spreadsheet you can extract the expressions which will include these body mesurement expressions also.
Does that part have standard geometry like block,cylinder etc.?
Are you certain about the material? Assigned to part geometry or not?
If part geometry is not standard, can you share the part file here? Will be easy to suggest you anything further.
The model has not standard geometry. Lots of features are managed by equations. I cant send it here, but for your imagination:
There are two parts at the picture. My expressions look like this:
I cant calculate volume from density and weight, because I designed only external surfaces of the part; in reality it consist more layers of material and system of cooling inside of the part - this is not important for me, i need to know only volume of shell.
Im trying to create a spreadsheets where i fill in a lenghts of parts to one collumn, than i click to update (or somethin like this) and in second column will be volume for each length.
One way it can be done is by using the 'Visual Report', Probably this will help. I have described this with an example and attached a video of the same process.
Assign some object name to the each solid body.
Set the selection filter to the 'Solid Body' > Select the solid bodies from UI > RMB > Properties > General tab > Enter name > Select 'Add index to name'. If you give name as 'Block_' and select add index to name then it will assign names Block_1,Block_2 etc. to the solid bodies. Note that these names will be different than those are present in the part navigator. You can assign different object name to individual solid body.
By default, the object names are off. You can turn it on.
Menu > Preferences > Visualization > Name/Borders tab > Part Settings: Show Object Names > Select the value 'All Views'. Assigned object names will be visible in UI.
Switch to 'HD3D Tools' navigator > Visual Reporting > Define New Report. Set the options as shown.
It will report the volume of each body. Note the name of bodies in the report, it's object names that were assigned initially. This can be exported to the spreadsheet. From there you can copy/paste in another excel and use it for the calculation you required.