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Sharing Parameters across Parts

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Message 1 of 13
Myoula
394 Views, 12 Replies

Sharing Parameters across Parts

I'm still learning, so forgive me if my terminology is off...is there a way to reference a parameter in the sketch of one part in the sketch of another part - what I'm trying to do is create a part that is always twice as long as another distinct part already in the assembly. Part B is always twice as long as Part A. I have renamed the dimension that controls the length of Part A (d0) to "Widget_Length" in the Parameters dialogue for Part A - now I want to make Part B's length parameter (which is also d0) be (2 * Widget_Length)
Using Inventor 11
Thanks,
Mike
12 REPLIES 12
Message 2 of 13
Anonymous
in reply to: Myoula

Mike:

Yes, it's possible.

You'll have to experiment a bit with derived parts. You can bring
across parameters this way. It might make sense to have one part
containing the parameter and the others derived from it.

It's a form of what many refer to as 'skeletal modelling'. Do a search
on the newsgroup for that term.

Richard

Michael Youla wrote:
> I'm still learning, so forgive me if my terminology is off...is there a way to reference a parameter in the sketch of one part in the sketch of another part - what I'm trying to do is create a part that is always twice as long as another distinct part already in the assembly. Part B is always twice as long as Part A. I have renamed the dimension that controls the length of Part A (d0) to "Widget_Length" in the Parameters dialogue for Part A - now I want to make Part B's length parameter (which is also d0) be (2 * Widget_Length)
> Using Inventor 11
> Thanks,
> Mike
Message 3 of 13
yannick3
in reply to: Myoula

Hi Mike
To transfer a parameter you can use derive part and before importing you must check the parameter you want to export in the prameter's window,on the derive part window choose parameter on the list (see attachment)
You can use too skeletal modeling (link)
http://www.sdotson.com/freetut/muscularmodeling.pdf
Sorry for my english
Yannick
Yannick Verreault
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Message 4 of 13
Anonymous
in reply to: Myoula

As Yannick and Richard say, derived parts will work if you haven't already
created the second part
If you have and don't want to recreate it, then you can create a spreadsheet
and import to both parts


wrote in message news:5568335@discussion.autodesk.com...
Hi Mike
To transfer a parameter you can use derive part and before importing you
must check the parameter you want to export in the prameter's window,on the
derive part window choose parameter on the list (see attachment)
You can use too skeletal modeling (link)
http://www.sdotson.com/freetut/muscularmodeling.pdf
Sorry for my english
Yannick
Message 5 of 13
Anonymous
in reply to: Myoula

Hi Mike,

I would sure like to know if you've succeeded in getting the software to do
what you want. I have a very similar problem, and have followed all the
advice I got, which matches what you also got. When working with parameters
I've found that I'm unable to get rid of references to files I've linked to
in the Parameter dialog interface (at the bottom). I've deleted the
spreadsheets, etc., and the linkage still exists. And I've been unable to
get one part to recognize features (holes or length dimensions) in another
part. I could manually create the locations and lengths, but that isn't the
way to supposedly take advantage of the software's features.

I wouldn't worry too much about the fact that "...(you're) still learning".
The Help files for the software are so poorly done that the best to be hoped
for in getting it to work for you is this forum. This situation has exited
for many years, and Autodesk refuses to make improvements. I'm sure it's a
money thing, you know, how much Autodesk can remove from you're employer's
(or your pocket) and place into their own via vaporware Help files, and
suggested high cost training seminars.

Anyway, I'd sure appreciate knowing whether you've successfully done what
you've asked about, and the process you took to succeed in doing so.

Wally

wrote in message news:5568290@discussion.autodesk.com...
I'm still learning, so forgive me if my terminology is off...is there a way
to reference a parameter in the sketch of one part in the sketch of another
part - what I'm trying to do is create a part that is always twice as long
as another distinct part already in the assembly. Part B is always twice as
long as Part A. I have renamed the dimension that controls the length of
Part A (d0) to "Widget_Length" in the Parameters dialogue for Part A - now I
want to make Part B's length parameter (which is also d0) be (2 *
Widget_Length)
Using Inventor 11
Thanks,
Mike
Message 6 of 13
rblawson
in reply to: Myoula

>>When working with parameters
I've found that I'm unable to get rid of references to files I've linked to
in the Parameter dialog interface (at the bottom).

Why do you need to delete them?

It sounds like you are linking the files rather than deriving them. Links can work one way OR two ways (e.g. change that file from this one), derives only work one way (changes in that file change this file).

>>And I've been unable to
get one part to recognize features (holes or length dimensions) in another
part

what are you trying to accomplish? If you're looking for a parameter, have you checked the "export parameter" box? This is a check box in the parameters window on the left side, and allows that particular parameter to be exported in either a link or a derive.

-Barrett
Message 7 of 13
nrg_drink
in reply to: Myoula

have you tried inserting the source ipt file, into the parameters box ??, do this in the same way you would link an xls sheet in but change the files of type to ipt, If I remember correctly you must have the parameters exported (tick box) for this to work properly
Message 8 of 13
Anonymous
in reply to: Myoula

Hi Barrett,

**Why do you need to delete them?

I always try to get rid of anything that seems to serve no purpose.

**Links can work one way OR two ways

I have a situation where the location of a hole feature on a part (A) is
dependent on the size of another part (B). Additionally, the hole in A
secures a part (C) to A, and C's location fits up against B. So I need to
describe this relationship in terms of the parameters of parts C and B.
Actually part C is a constant, so I don't really need to include a parameter
from its definition. I thought I should be able to include the parameters
of part A, but I've not been able to find any way to link them, even though
the online Help suggests that you should be able to develop parameter files
that are available to other parts.

I guess that's my main question. Does what the online Help states,
concerning the availability of parameter files to other parts (Excel) really
exist, or am I chasing vaporware? The parameter file name and path (let's
call it "ABCparameters.xls") is listed in gray at the bottom of the file's
Parameter window. However it doesn't seem to serve any purpose, as the
parameters contained within the file are not on the list of the many
parameters of the currently opened file. So how can I make use of an
expression that defines the location of the hole in part A? Into this mix
is the fact that the final assembly is an iAssembly, so I need the
parameters to define a changing set of hole locations.

**It sounds like you are linking the files rather than deriving them. Links
can work one way OR two ways (e.g. change that file from this one), derives
only work one way (changes in that file change this file).

I have looked at deriving the hole location from the size of the other
part. Since this is an iAssembly, with other versions, I'm not sure I could
make that solution work.

**what are you trying to accomplish? If you're looking for a parameter,
have you checked the "export parameter" box? This is a check box in the
parameters window on the left side, and allows that particular parameter to
be exported in either a link or a derive.

I have accessed the "export parameter" box". That is why I created the
ABCparameters.xls file. That may be the problem. I formed it exactly as
the other IPT files that use an Excel file (ie, columns containing Member,
Part No., followed by the parameters I want to access from other file(s).
Rows containing versions. Initially I only used one version to see if that
would work. It didn't.
I'm not sure what you mean by the check box in the parameters window on
the left side. There is only one check box in this window. It says:
Display only parameters used in equations. Below that are two buttons: Add,
Link. If I hit the Link button, it says that it is a duplicate to an
existing link. That is a true statement, but the parameters in the linked
file are not shown in the list.
If you are referring to the checkboxes in on "Export parameters" list,
I've tried exporting these parameters to a file. The problem is they don't
show up in the Excel file. They do show up in the files iProperties window
under the Custom tab, showing they were "Exported"??, but to where is
unknown.

SO WHY CAN'T I SEE THE PARAMETERS IN THE FILE I'VE LINKED TO??? If this is
a formatting issue, in regard to the way the rows, columns of the Excel file
are placed, I have no model from the online Help to show me how this file
might be any different from the 3rd party Excel file that works with my
iParts and iAssemblies.

Sorry if I've been a bit long winded in my explanation, but I wanted to make
sure you could understand the issue. Thanks so much for answering my post.

Wally


wrote in message news:5569109@discussion.autodesk.com...
>>When working with parameters
I've found that I'm unable to get rid of references to files I've linked to
in the Parameter dialog interface (at the bottom).


It sounds like you are linking the files rather than deriving them. Links
can work one way OR two ways (e.g. change that file from this one), derives
only work one way (changes in that file change this file).

>>And I've been unable to
get one part to recognize features (holes or length dimensions) in another
part

what are you trying to accomplish? If you're looking for a parameter, have
you checked the "export parameter" box? This is a check box in the
parameters window on the left side, and allows that particular parameter to
be exported in either a link or a derive.

-Barrett
Message 9 of 13
Anonymous
in reply to: Myoula

HInrg,

I just tried this by dragging the file into the Parameters window. I got a
message that said I must use Derived parts or Derived assemblies. I'll have
to get back to you after looking into this further. Derived parts appear as
dumb solids, unless you double click on them in the browser. So I'm not
sure how that might give me the parameters I need from the original file.

Following your method there no way to Link the file through the parameters
window, since there was no files of type option for ipt, only xls and All
files. The message it gave me was the same as the one I mentioned above.
I'm not sure where this Derived parts solution may be leading, so I'll have
to get back to you later when I attempt using Derived parts instead.

Wally

wrote in message news:5569191@discussion.autodesk.com...
have you tried inserting the source ipt file, into the parameters box ??, do
this in the same way you would link an xls sheet in but change the files of
type to ipt, If I remember correctly you must have the parameters exported
(tick box) for this to work properly
Message 10 of 13
rblawson
in reply to: Myoula

Wally,

It seems you're missing the basic procedure, so i'll try and walk you through it and then address your questions in more detail.

FIRST THINGS FIRST: Check parameters for export.
Any parameters in part A that you want to access in part B need to be checked for export. There is a check box on each parameter's row between "model value" and "comments" (it's on the right, I said it was on the left before, sorry).

TO LINK PARAMETERS between inventor files:
click the "LINK" button, select file type: all files, browse to the file for part A and click "Open". any parameters that have been checked for import as above will be included.

TO EMBED or LINK PARAMETERS from excel files:
click he "LINK" button, browse for your excel file, check the link or embed radio buttons, specify the start cell, and click OPEN. It is important that the excel file be formatted in a particular manner: The parameters must be on the first sheet, starting at the cell you specify, with order: (name) (value) (units) (comment). units and comment are optional and the cell must read as it would in inventor's parameter window. inventor only looks at the cell's value.
"Link" will bring the values into the model, and can be used in different inventor parts, use it where the spreadsheet is the controlling factor. "Embed" allows inventor to change the values of the cells, use it if you want to use the spreadsheet for output.

TO DERIVE PARAMETERS BETWEEN PARTS:
Check appropriate parameters for export as above for part A. Open part B, select "derive component" in the panel bar. Expand the exported parameters folder, and select the exported parameters you want by clicking on them. Yellow+ brings them in, Grey- leaves them out. You can tell it to always bring in any new ones on update by setting the Yellow+ for the "exported parameters" line, or only the ones you select by leaving it half yellow half grey as in the attached picture.

RELEVANT HELP FILES:
"Use a parameters spreadsheet"
"Learn about parameters" >>How are linked parameters used?
"Parameters reference" >>Link >>Exported parameters column
"Use parameters in a model" >>Define parameters in a spreadsheet and link to a part or assembly
"About derived parts and assemblies"
"Tips for creating and using derive parts" >> Exporting parameters
"Derived part reference"


-Barrett
Message 11 of 13
rblawson
in reply to: Myoula

Wally -

ok, apologies if the walk through was heavy handed, but I have a better understanding of your problem now.

You were expecting that when you export parameters and then link to an excel file, that the parameters will be put in the excel file, right? While that might seem logical, the information flows from excel to inventor. There are various reasons to want to do this - you already have stuff calculated in Excel, or it's easier to create equations in excel, etc.

two things you ran into:
1) formatting for iPart tables is different than formatting an excel sheet for parameters. (parameter name) (value) (unit) (comment), as above.
2) to delete a linked folder: in parameters window, right click on the folder and select delete. Might not let you do it if a parameter in the folder is in use.

so for what you want to do, which is to take information from one file and use it in another, you want to derive the information. Note that you don't have to derive the solid lump of the derived part if you don't want to, you can derive just sketches, work planes, etc.

When you start obsessively deriving things, it is called "skeletal modeling". You said that just deriving parameters might not work for you, so you might look into deriving a sketch from one part to the other. In order to derive a sketch, it must be visible in the first part when you start the derive command in the second part.

-Barrett
Message 12 of 13
Anonymous
in reply to: Myoula

Hi Barret,

Thanks for the detailed input. I appreciate the time you spent to provide
it. I'll have to take a little time to go through your suggestions to see
what works. Then I'll return with the results.

Wally

wrote in message news:5570470@discussion.autodesk.com...
Wally -

ok, apologies if the walk through was heavy handed, but I have a better
understanding of your problem now.

You were expecting that when you export parameters and then link to an excel
file, that the parameters will be put in the excel file, right? While that
might seem logical, the information flows from excel to inventor. There are
various reasons to want to do this - you already have stuff calculated in
Excel, or it's easier to create equations in excel, etc.

two things you ran into:
1) formatting for iPart tables is different than formatting an excel sheet
for parameters. (parameter name) (value) (unit) (comment), as above.
2) to delete a linked folder: in parameters window, right click on the
folder and select delete. Might not let you do it if a parameter in the
folder is in use.

so for what you want to do, which is to take information from one file and
use it in another, you want to derive the information. Note that you don't
have to derive the solid lump of the derived part if you don't want to, you
can derive just sketches, work planes, etc.

When you start obsessively deriving things, it is called "skeletal
modeling". You said that just deriving parameters might not work for you,
so you might look into deriving a sketch from one part to the other. In
order to derive a sketch, it must be visible in the first part when you
start the derive command in the second part.

-Barrett
Message 13 of 13
RobSinglehurst
in reply to: Myoula

Ray,
That's not strictly true when just deriving parameters into another part. Parameters and sketches can be derived into any existing part. It's only 3D solids that can't be.

Cheers,

--Rob Singlehurst
Cheers,
--Rob
Inventor 2024.2

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