table displays equation instead of value

[billco-mfg]

I'm detailing an iPart. Only two dimensions need to be included in the table. One is the driving dimension and the second is a function of the driving dimension. How do I get the column for the second dimension to display a value, rather than an equation?

[billco-mfg]

I figured out a way, but I wonder if there is a simple formatting option.

I added all the parameters involved in the equation to the iPart table. Then I replaced the equations I had in Inventor with Excel equations. This is a messy solution, since it forces you to add a bunch of otherwise unnecessary columns to the ipart table.

[daveyfinchy]

Hi
Have you found a solution yet?
I've got a similar problem where a dimension I want to show on the drawing is not an actual perameter, but a formulated value based on a few perameters.

Don't quite understand your suggested solution? Can you explain it more, thanks.
Dave

[dan_inv09]

If the second parameter is driven by the first, why does it need to be in the table? You only change/pick the first value, right?

[billco-mfg]

The overall length of the part is a function of another dimension. I need to show the OAL on the drawing, so I need it to appear in the table.

[billco-mfg]

I think I'll need to keep using the method I posted.

Before the part was an iPart, there was a parameter defining the length of an opening (B). Another parameter defined the overall length of the part (A, where A = B+4).

When I detailed the part, I decided that I needed to show two dimensions in a table, OAL and OpenWidth. When I added A to the table, the values displayed a 'A+4' insteadd of just showing the resulting value. If I edited the table via Excel and did the math inside the Excel cells, then just the value appearrs in the table.

[dan_inv09]

Ahh, I missed "detailing," didn't read carefully enough.

How are you making your table? If you just put the spreadsheet on the drawing, how do you handle all the extra stuff inventor needs in the column headers?

Have they improved the way inventor deals with spreadsheets in drawings? I gave up trying several releases ago.

[billco-mfg]

There is a table command now that lets you select an iPart or iAssembly table as the data source. Once the table is placed, you can format/select the columns and hide rows.

[dan_inv09]

Despite the screen name I am using 2008.
I've played with the new table command a little. It has some potential but now this is another limitation.

[billco-mfg]

I don't know if it is a limitation or if I'm just unaware of the simple solution.

[Anonymous]

A much simpler approach would be to add a driven dimension to the part,
either in the originating sketch, or in a separate sketch. Reference
dimensions may be added to underconstrained geometry at any time by
selecting General dimension, then the Driven Dimension Toggle at the upper
right of the screen. Then your iPart and Table should format correctly.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows Classic Theme
http://teknigroup.com

[Anonymous]

The first post contains an R2008 ipt/idw example..... here's an image of the
resulting table.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows Classic Theme
http://teknigroup.com

[billco-mfg]

Dim B is in a sketch, but dim A is the length of an extrusion. I don't think there is a way to apply your method to simplify what I already have.

I'll have to remember that though. It would work out in many cases.

[Anonymous]

Create a new sketch parallel to the extrusion. Project the reference edges
and add a driven dimension to the ref edges. Turn the sketch visibility off
after creation.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows XP Silver Theme
http://teknigroup.com

[billco-mfg]

I don't think that would simplify what I have, but it's a good method for other models.

Originally, I was hoping there was a display as value/equation option I missed.

[Anonymous]

Unfortunately, there is no option for that.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows XP Silver Theme
http://teknigroup.com

[billco-mfg]

I have another part that might allow me to apply your method, so I just took a look at your example. The one thing I don't understand is how you add the reference parameter to the table. They don't appear on the parameter tab of the iPart author window.

[Anonymous]

1. Make sure the Reference is marked for export.
2. In iPart Author, select the properties Tab. The reference should now be
there. (see attached)

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows XP Silver Theme
http://teknigroup.com

[billco-mfg]

OK I got it to show up. The properties tab is an odd place to put that.

When I add the driven dimension to the table, I run into the next problem. The entire column shows the same value. They only seem to update as I activate each member, which would cause some problems when the part is changed.

[mcleamic]

How do you mark the reference for export?

I am using IV11 SP3.

Nevermind, I figured it out. Message was edited by: mcleamic