Need Reliable Excel Driven Sheet Metal Assembly Workflow

[kbodoh]

I design many sheet metal assemblies that look like 4-6 sheets with edge treatments (hem, flange,...). These are fastened together by rivots, screws or welds. Many of the sheet metal faces meet at non-perpendicular angles that change when my Excel spreadsheet changes. Here is what I have tried:
1. Build parts in assembly by constraining and adapting flanges to other faces. Problem is how to apply 3 constraints to lock a sheet in place prior to knowing and constraining the flanges to neighboring sheets. All assemblies blow up (red crosses) when Excel is changed.
2. Make work planes and one base face per sheet metal part. Sketch faces for flanges onto neighbor sheets and project geometry. Create bend to join faces. PROBLEM: Assembly blows up when Excel changes. Best fix is to define the flange faces using a work plane with the origin axis defined on the future bend line.
3. Skeletal modeling fails since derived parts must be constrained together in an assembly. It is almost impossible and very unstable to apply 3 constraints to a sheet metal part to lock it in position.
4. Create a block representing the basic shape of the assembly. Use the faces of the block to project and define sketches for faces. Adapt the flanges to the block to get proper angle. PROBLEM: Projected geometry often fails to follow when the block changes. Flanges often blow up when block geometry is changed.

ALL THE ABOVE methods fail to give me necessary idw dimensions. The geometry and dimensions of the base face is often necessary in idw to layout cut lines on sheet metal and verify final dimensions. The best fix is to create offset flanges with no relief. This preserves the corners of the base face for the idw dimensions and assembly constraints.

THE ONLY WORKING WORKFLOW I FOUND:
A. Create an Excel table of parameters defining the block (basic shape of the final assembly).
B. Calculate all angles between faces of the block in excel (best by calculating all XYZ coordinates of base face corners and using vector math to calculate angles)
C. Draw sketches on XY and XZ planes where all dimensions are derived from Excel (Problem: All dimensions must alway be positive)
D. Extrude sketches to make block.
E. Create base faces by sketches drawn and extruded off sides of block. Do not apply any constraints and do not drag any parts. Once dimensions are set, ground all parts.
F. Create offset flanges by deriving proper angles from Excel (Link same file into all parts)
G. Create all drawings necessary.
H. Save as a read only model.
I. Pack&Go into new project, rename Excel, DA rename ipt idw iam, resolve to new Excel file
J. Edit Excel
K. Review Block.ipt, other ipt and iam to verify changes took
L. Fix idw detached dimensions and refresh parts list
TOTAL Time 30-60 minutes per assembly.

I think it is foolish to have Excel do calculations that Inventor should manage, but Inventor is really slow, blows up and crashes using other work flows. Inventor should be able to manage changing a 4-6 sheet assembly in 5-10 minutes where most of the time is polishing up idw for readability.

Have I missed something?

[MechMan_]

Have you looked into the Master Sketch design method?



MechMan

[Anonymous]

#3: It was my understanding, when you do skeletal modeling, you just need to
bring the part in the assembly and ground it. You should not need to constrain
the parts together if they are derived from 1 master model/sketch.

--
Dave Jacquemotte
Automation Designer

[MechMan_]

Thanks Dave. Somehow missed that.



kbodoh, when using the Master Sketch (skeletal) approach you don't have to constrain the part in the assy. The master sketch dictates the part's placement in space. After you insert a part created via the Master Sketch approach into an assy RMB on the part => Properties => Occurence tab and set the XYZ locations to zero and then ground the part. Better yet use Kent's Insert & Fix program (http://www.mymcad.com/KWiK/iCode/icode.htm).

MechMan

[Anonymous]

Why are you applying constraints in a master sketch assembly? You should not need to.
--
Kent
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"kbodoh" wrote in message news:f160fd4.-1@WebX.maYIadrTaRb...

> 3. Skeletal modeling fails since derived parts must be constrained together in an
assembly. It is almost impossible and very unstable to apply 3 constraints to a sheet
metal part to lock it in position.

[kbodoh]

Thanks. I must have missed that.

If I build a box where the top and bottom are parallel planes but the sides are not perpendicular to any other side, top or bottom, I need the angles calculated between planes (12 total between sides, top bottom). I will create flanges at the edges of the sheet bent to these angles. Don't I need to create 12 sketches on work planes perpendicular to the common axis of each pair of sides and measure the angle in a driven dimension? Or do I create sketches for additional faces and add the bends (instead of flanges)? Driven dimensions don't update reliably and bends blow up (red crosses) when base geometry is changed. What is the best workflow?

[Anonymous]

I am not sure I follow all of what you want, but I made up a simple example of a way to
use a master sketch. Look in IVCF for Angle box. From the point I left it you would have
to start adding planes to sketch on to complete it. Most times I make sketches that
extrude as faces and in the face dialog pick the edge to add the bend to. You basically
have to forget about the flange tool.

--
Kent
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"kbodoh" wrote in message news:f160fd4.4@WebX.maYIadrTaRb...
> Thanks. I must have missed that.
> If I build a box where the top and bottom are parallel planes but the sides are not
perpendicular to any other side, top or bottom, I need the angles calculated between
planes (12 total between sides, top bottom). I will create flanges at the edges of the
sheet bent to these angles. Don't I need to create 12 sketches on work planes
perpendicular to the common axis of each pair of sides and measure the angle in a driven
dimension? Or do I create sketches for additional faces and add the bends (instead of
flanges)? Driven dimensions don't update reliably and bends blow up (red crosses) when
base geometry is changed. What is the best workflow?
>

[kbodoh]

Check out my TranD01 file in IVCF. This works but Excel drives through parameters. Setting up a model like this takes alot of work. Then I have to Pack&Go, change file names, resolve links, update driven dimensions, and clean up the drawings. Do you have experience working with non-perpendicular sheet metal parts like this? I am afraid that skeletal modeling will require many work planes and sketches -- all capable of failing during update.

Thanks, Keith

[Anonymous]

Keith

It complained about some things missing when I opened it, but it all appears there. I
agree that method does look like a lot of work. I don't even know where to start editing
it without causing it to blow up.

For something like this instead of using the wireframe method like I posted, start a part
file and make a part the shape of the inside of the duct. Then derive this into the new
sheetmetal files as a surface and build the sheets on the surface, and reference the
surface edges for the SM edges. If you change the core model then the SM parts will also
change. There have been a couple examples of this posted to customer files in the past.
Not sure if they are still there or not.

--
Kent
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"kbodoh" wrote in message news:f160fd4.6@WebX.maYIadrTaRb...
> Check out my TranD01 file in IVCF. This works but Excel drives through parameters.
Setting up a model like this takes alot of work. Then I have to Pack&Go, change file
names, resolve links, update driven dimensions, and clean up the drawings. Do you have
experience working with non-perpendicular sheet metal parts like this? I am afraid that
skeletal modeling will require many work planes and sketches -- all capable of failing
during update.
> Thanks, Keith
>

[Anonymous]

Keith, You already have a part (called TranD01-Block) that could serve as
the
base for four derived parts, like Kent describes below. You should be able
to
completely dispense with the Excel spreadsheet.

The "included angle" between the arbtrarily oriented planar faces can be
found
by setting up a plane that is normal to the two planes. Then you can project
the
two planes to a sketch you set up on the plane you created, and define an
angular dimension between the two lines. (It seems that you need these
angles
for sheet metal bends).

You could create all these driven angular dimensions in the base part
mentioned
above and export them to the 4 derived parts.


"Kent Keller" wrote in message
news:79D5DB552FE03F31E0C4AB1020063AAF@in.WebX.maYIadrTaRb...
> Keith
>
> It complained about some things missing when I opened it, but it all
appears there. I
> agree that method does look like a lot of work. I don't even know where
to start editing
> it without causing it to blow up.
>
> For something like this instead of using the wireframe method like I
posted, start a part
> file and make a part the shape of the inside of the duct. Then derive
this into the new
> sheetmetal files as a surface and build the sheets on the surface, and
reference the
> surface edges for the SM edges. If you change the core model then the SM
parts will also
> change. There have been a couple examples of this posted to customer
files in the past.
> Not sure if they are still there or not.
>
> --
> Kent
> Assistant Moderator
> Autodesk Discussion Forum Moderator Program
>
> When posting Attachments Please Zip first and Use the new IVCF
> Web http://discussion.autodesk.com/WebX?14@186.Fx3taaT3ofu.79@.f15ad3a
> Newsreader
news://discussion.autodesk.com/autodesk.inventor.customer-files
>
> "kbodoh" wrote in message
news:f160fd4.6@WebX.maYIadrTaRb...
> > Check out my TranD01 file in IVCF. This works but Excel drives through
parameters.
> Setting up a model like this takes alot of work. Then I have to Pack&Go,
change file
> names, resolve links, update driven dimensions, and clean up the drawings.
Do you have
> experience working with non-perpendicular sheet metal parts like this? I
am afraid that
> skeletal modeling will require many work planes and sketches -- all
capable of failing
> during update.
> > Thanks, Keith
> >
>
>

[kbodoh]

I am rebuilding my model as Kent and you suggest. I need to prove that this workflow will not fault with failures in creating faces and flanges. In the past I have had sketch planes fail to move, flange faces fly off into space, projected geometry fail to update, bends fail due to relief intersection on the faces, and many other mysterious red crosses. Oh.. and sketch lines which snap to the wrong location just because there are always two solutions to any dimension placed on a sketch.

I see one pitfall with measuring angles with driven dimensions. I believe these fail to update when the parameters or Excel are changed. I believe that I need to edit each sketch to update these dimensions. Is this correct?

I have decided to drive my designs from Excel because everything our company makes is custom. I expect soon my Excel table parameters will be driven by additional calculations done in a master Excel table or database. Is this an acceptable workflow with Inventor? I do have problems renaming parts and the Excel table with job number names. It seems that the link must be verified everytime I open a part. Is there another way to rename the iam, ipt, idw, xls for all files in a project (after Pack&Go)?

[kbodoh]

I inserted a part when I was in isometric view. Setting the XYZ to 0 did not change the angles (as expected). The angles are not available. I added flush constraints between origin planes to fix the problem. Is there an easier method? Does Kent's Insert&Fix program deal with the angles correctly?

[Anonymous]

When you derive the part in, the origin should already be set where it needs to
be (origin of assembly should be origin of part). You just need to ground the
part. And yes, Insert&Fix does this automatically.
If you are going to use Skeletal Modeling, I&F is a must have. (IMO)

--
Dave Jacquemotte
Automation Designer

[Anonymous]

Have you tried just sharing parameters via the derive method rather than relying on Excel?
I don't think I have resorted to using Excel since starting to use the Master Sketch
method.

As far as inserting parts using a master sketch method, I really do think Insert n Fix
helps a lot. Often times I will throw away a whole assembly and rebuild it in seconds
using it just to adjust the order of parts in the browser or something along those line.
Everything coming in using the same origin is part of the beauty of Master sketches.

--
Kent
Assistant Moderator
Autodesk Discussion Forum Moderator Program


"kbodoh" wrote in message news:f160fd4.9@WebX.maYIadrTaRb...
> I am rebuilding my model as Kent and you suggest. I need to prove that this workflow
will not fault with failures in creating faces and flanges. In the past I have had sketch
planes fail to move, flange faces fly off into space, projected geometry fail to update,
bends fail due to relief intersection on the faces, and many other mysterious red crosses.
Oh.. and sketch lines which snap to the wrong location just because there are always two
solutions to any dimension placed on a sketch.
> I see one pitfall with measuring angles with driven dimensions. I believe these fail to
update when the parameters or Excel are changed. I believe that I need to edit each sketch
to update these dimensions. Is this correct?
>
> I have decided to drive my designs from Excel because everything our company makes is
custom. I expect soon my Excel table parameters will be driven by additional calculations
done in a master Excel table or database. Is this an acceptable workflow with Inventor? I
do have problems renaming parts and the Excel table with job number names. It seems that
the link must be verified everytime I open a part. Is there another way to rename the iam,
ipt, idw, xls for all files in a project (after Pack&Go)?
>

[Anonymous]

Kbodoh,

You are not alone. (IV6 user) I am also trying to get things working with Excel for much the same reasons you are.

I too have to verify the Excel link every time I open an iam. (The title of the excel file in the browser does not match the actual file that it is linked to!)

If I point to one master excel file - all the other assemblies that reference that file - get the current parameters. (The excel file format is done with a look up table so that IV can read it!)

One solution is to select the version I want in the excel file and then drop it into the folder with the rest of relative files and point to that. The problem for me is that there are multiple copies of the original file which is no good for global updates on the system so this doesn't work for us.

FYI. I also had a problem with ipt files retaining old links to previous excel files. The only way to correct, BTW sincere thanks Kent, was to make a copy of the file with a new name or make it an ipart.

I've got a work around, but it too is not efficient and need something better.

I'll stop here...

Regards
Ron