linkage of unigraphics with excel.

[dhaval082]

Dear

I have made one piston rod in unigraohics, now i want to connect all dimensions of piston rod into excel sheet..
now whenever i required to change any dimension of my piston rod i will change into excel sheet and the effect i will see in the model of piston rod.

Reply as soon as possible..

 

[MickyV007]

Have a look at Family tables or deformable parts, use command finder if you can't locate the features.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit (Intel(R) Xeon(R) CPU X5650 @2.67GHz)
24.0 GB
NVIDIA Quadro 4000 + NVIDIA Tesla C2050

 

[rc0213]

Depending on what you are trying to do, but if it is to create a part you can change through a table, I normally use Part Family. Go to

Tools, Part Families...

 

[dhaval082]

My Objective is to make a piston and all the dimensions of piston will appear in the excel sheet...now this excel sheet which contains all the dimensions of piston has to be link with unigrphics..now whenever i required dimension change,i will change only into excel sheet and corrosponding effect will appear in model...

 

[JohnRBaker]

And why are you having problems with this? NX has been able to do this for years. There are functions in the expression system which will allow you to read/write from/to the cells of an external spreadsheet.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[dhaval082]

in expression function shows only refresh external spreadsheet but not give how to connect external spreadsheet to the ug.
please send me the step by step procedure

 

[RobLN]

Hi dhaval082

I have some experience with this. Its always useful to know what NX you're running but for the record this advice is based upon me using NX 7 1/2 + TeamCenter

So Part families:

1. Make a 3D part with the major dimensions defined with an expression (eg. Piston Diameter=50 , Piston length=100 and so on) This is the master part.

2. Make a 2D drawing of the 3D part (I use embedded style - so no separate drawing file please...)

. Tip: Tie your dimensions to the geometry so that when the shape grows the dimension goes with it - to do this see dimension -> origin.

3. In the 3D model select tools-> part families (PF)

(Now we'll tie the 3D to the XL.)
4. Switch the exportable part family off (this causes some problems in my experience..)
5. In the PF dialog you'll see a load of expressions (once you choose it in the drop down..) within that list you should see the ones you created as well as the system generated and default ones. Now choose your important expressions for your part and highligh it in the list (go 1 by 1)
6. With your expression highlighted click add column button. Repeat as needed.
. What this does is builds your 'linked' XL in the background
7. Once you're happy you have all the expressions you need hit edit button
8. System will transfer you to excel.
9. Now you'll see the expressions transferred to columns in your XL
10. Now play and you can re-assign new values to drive the 3D model. Use the tools in the 'add ins' to assign your new part numbers and create your 'family members' based upon your master part. I usually run in the following order: 1 assign no's, 2 apply values (check - NB line by line only), 3 Create parts, 4. Update parts 5 Save.
Hope some of this helps.

If anyone can advise how I can get the output of a conditional expression (which I can't seem to choose in the columns) into the XL file that would help me out a lot

Thank you

RLN.
.

Solid Edge; I-Deas 7 to 12; NX4, NX5 NX6 & currently NX7.5 / TeamCenter 8.3 Windows XPpro 3GB

 

[dhaval082]

in aboved threads how to apply create a part and apply a part

 

[RobLN]

To Apply a part you need to do the following:

From the Master model for the family in (Modeling mode)

Tools > part Family > Edit

Now you're transferred to XL by NX automatically.

When you use XL through NX you get a new menu on the far Right hand side called 'Add-ins' (I use XL 2010)

Click on this and you gat a sub menu called Part Family / menu commands and there is a drop down on the right hand side of it.
If you click on the drop-down arrow you get to see the following options:

Verify
Apply
Update
Create
Save
Assign
Cancel

So for 'create' highlight as many data lines in the XL sheet that control the model as you want to create (NB you must first assign the part numbers!) and then just click on the 'create' from the Part family sub menu to create.

Note I find that the machine tends to run out of memory above about 100 lines at a time.
For apply its the same as create except you can't do multiple lines and you have to go line by line. Hope this helps !


RLN
Update


Solid Edge; I-Deas 7 to 12; NX4, NX5 NX6 & currently NX7.5 / TeamCenter 8.3 Windows XPpro 3GB

 

[dhaval082]

what is the option in ug for connect excelsheet using vb.net

 

[jerry1423]

Have you done a search in this forum on this topic?
You may find the answers that you are looking for.

 

[dhaval082]

sir i have made Template in nx6 .and excel calculation for the same Template.so now required to connect excel calculation with the template using C#.net so how to connect this?

 

[dhaval082]

I created an excel spreadsheet with all different calculations and also create template in nx now i make interface between the excelsheet and template now i required that whenever i change the excelsheet automatic nx model will be change so how to nx model link with excelsheet