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Wojtek Weber
Guest
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 Posted:
Thu Apr 28, 2005 8:10 am Post subject:
How to add driven dimension into the family table |
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I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
Thanks in advance.
Wojtek
WF1
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GWDavis28
Joined: 08 Apr 2005
Posts: 70
Location: Massachusetts
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| Posted:
Thu Apr 28, 2005 12:23 pm Post subject:
re:How to add driven dimension into the family table |
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Wojtek, did you add the feature of the unbend into the table? We use the Flat State command under the sheet metal menu manager to create our flat states and it work really well. Your also trying to add a driven parameter right and not a created one? If the parameter is in the drawing only, then you can not add it into the family table.
Hope this helps, Glenn |B) |
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David Janes
Guest
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| Posted:
Thu Apr 28, 2005 4:10 pm Post subject:
Re: How to add driven dimension into the family table |
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"Wojtek Weber" <wweber@gazeta.pl> wrote in message
news:d4q297$et1$1@inews.gazeta.pl...
| Quote: | I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
|
I can think of two ways you could make a parameter that you could include in the
table and whose value you could use in a repeat region. But in both cases they'd
be derivative, measures, calculated values and wouldn't control anything. So the
purpose of putting such in a table is a little obscure. You could certainly create
these parameters and use their values in a table or drawing without putting them
in family table.
* Create a parameter ('Tools>Relations') by assigning it the sum of the values of
all the features which produce the length, e.g., t_length=d5+d8+d10. This will
work if these feature dimension variables remain the same within an acutal family
of parts.
* Create a measure feature ('Insert>Model datum>Evaluate') and use this to create
a parameter containing/recording this value.
David Janes
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Wojtek
Guest
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| Posted:
Fri Apr 29, 2005 4:10 pm Post subject:
Re: How to add driven dimension into the family table |
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Thanks for answer. The reason I need additional dimension of the flat
part is very simple. Quality department needs documentation containing
this dimension. So I'm adding it into the simple drawing of a flat part
(flat state). But I'm not able to create the table containing this
dimension (or better dimensions) in the family of the parts. Of course
it is possible to create parameter as you've described. This is known
feature. Anyway for more than two bends it produces formulas which are
very complex and difficult to maintain. So I've started to search the
easier solution.
The second solution is unknown for me. I haven't got `Evaluate` under
'Insert>Model datum>` menus. I'm using WF1
Wojtek |
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Wojtek
Guest
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| Posted:
Fri Apr 29, 2005 4:10 pm Post subject:
Re: How to add driven dimension into the family table |
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Thanks for explanation. It makes me sure I'm doing all the work
correctly, but I don't know some tips and tricks (if they exist).
I'm using Flat State command and later create two model drawing. It
means there is a complete, bent detail and Flat State on it. Standard
dimensions shown on the drawing (view) of the flat state are not
acceptable to me. So now I'm simply adding needed dimensions and hiding
the other ones. Of course added dimension do not control anything. But
they are important for control purposes during manufacturing. It works
OK for one detail.
Now I'm creating family of basic i.e. bent details. Flat state for the
other details from family are created automatically. And so I'd like to
have not only dimension from model, but this added dimension grouped
into the table and assigned into the particular family member on the
table. I also desire this dimension changes automatically when some
changes are introduced into the generic and/or the family table.
Hope it's understandable.
Anyway, I'm afraid this feature is only desire. Am I right? Or any
simple solution exist?
Wojtek
GWDavis28 wrote:
| Quote: | Wojtek, did you add the feature of the unbend into the table? We use
the Flat State command under the sheet metal menu manager to create
our flat states and it work really well. Your also trying to add a
driven parameter right and not a created one? If the parameter is in
the drawing only, then you can not add it into the family table.
Hope this helps, Glenn |B)
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Wojtek
Guest
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| Posted:
Fri Apr 29, 2005 4:10 pm Post subject:
Re: How to add driven dimension into the family table |
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|
Thanks for answer. The reason I need additional dimension of the flat
part is very simple. Quality department needs documentation containing
this dimension. So I'm adding it into the simple drawing of a flat part
(flat state). But I'm not able to create the table containing this
dimension (or better dimensions) in the family of the parts. Of course
it is possible to create parameter as you've described. This is known
feature. Anyway for more than two bends it produces formulas which are
very complex and difficult to maintain. So I've started to search the
easier solution.
The second solution is unknown for me. I haven't got `Evaluate` under
'Insert>Model datum>` menus. I'm using WF1
Wojtek |
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GWDavis28
Joined: 08 Apr 2005
Posts: 70
Location: Massachusetts
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| Posted:
Sat Apr 30, 2005 10:34 pm Post subject:
re:How to add driven dimension into the family table |
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Wojtek,  Sorry man yah this is not possible. Created dimensions (dimensions added into a drawing) can not be used in a family table to drive/change models.
As an alternative, you could always create your parts in the flattened state get the driven dimensions you are looking for and then add those to the family table.
I guess it all depends on what's most important to you. The parameters/driven dimensions or the flattened state or the formed state.
You could with some work create the family in the flat state and have all of the driven dimensions for both states so that they can appear in the table. But you'd have to look at the parts and determine what can be made commonly. Though it's easy for me to talk since I don't know what your parts look like.
Anyway, good luck and let me know if I can help with anything else.
Later, Glenn |B) |
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Ron M.
Guest
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| Posted:
Sun May 01, 2005 12:10 am Post subject:
Re: How to add driven dimension into the family table |
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"Wojtek Weber" <wweber@gazeta.pl> wrote in message
news:d4q297$et1$1@inews.gazeta.pl...
| Quote: | I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
Thanks in advance.
Wojtek
WF1
|
You can test out the following technique to see if it provides you with what
you're looking for here.
1) Retrieve the flat state instance and add Part mode Reference Dimensions
to it. In Wildfire you can create Part or Assembly mode Reference Dimensions
two different ways. The first way is to choose Edit - Set Up - Ref Dim. You
will have to select a datum plane for the dimensions to be parallel to. The
second way is to add what is known as an Annotation feature Ref Dim in
Wildfire 1 or 2. There's an icon on your Wildfire toolbar for Annotations.
This approach also requires the user to select a datum plane for their Ref
Dim to be parallel to. After you have created the first Ref Dim you can then
select this Ref Dim to orient the part for subsequent Ref Dims' creation.
Once you have your Ref Dims created, perform a Switch Symbols operation so
that you can see the Ref Dims' Symbol Names. Such as rd0 and rd1, as
examples only. You can also do this by choosing Tools - Relations.
2) Retrieve the generic model and choose Tools - Family Table. Click on the
icon for adding dimensions, features, etc. and choose the option named
'Other'. Pro/ENGINEER will prompt you to enter a Symbol Name. This is where
you can enter the rd0 and rd1 or whatever your Ref Dims Symbol Names turn
out to be after having created them in the flat state instance.
This should solve your problem. You can also use the 'Other' option to
include dimension tolerances in a Family Table. Not that there is much of a
demand for this type of thing, but I thought that I would offer that up to
you while I am discussing the 'Other' option in Family Tables.
Ron M. |
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Wojtek Weber
Guest
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| Posted:
Fri May 06, 2005 4:00 pm Post subject:
Re: How to add driven dimension into the family table |
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Thanks a lot for the information. It works, but not solves the main
problem. I've checked it doesn't work because Flat State became part of
a family table. You can add ref dimension into the family name, but they
are not updated when model is changed.
Anyway all the information I've received from you and from other guys is
extremely useful to try to solve the main problem by myself.
Seems ProE do not allow to create really useful family table for Flat
State in simple way. The only way is to create some parameters and
relations.
Wojtek
Ron M. wrote:
| Quote: | "Wojtek Weber" <wweber@gazeta.pl> wrote in message
news:d4q297$et1$1@inews.gazeta.pl...
I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
Thanks in advance.
Wojtek
WF1
You can test out the following technique to see if it provides you with what
you're looking for here.
1) Retrieve the flat state instance and add Part mode Reference Dimensions
to it. In Wildfire you can create Part or Assembly mode Reference Dimensions
two different ways. The first way is to choose Edit - Set Up - Ref Dim. You
will have to select a datum plane for the dimensions to be parallel to. The
second way is to add what is known as an Annotation feature Ref Dim in
Wildfire 1 or 2. There's an icon on your Wildfire toolbar for Annotations.
This approach also requires the user to select a datum plane for their Ref
Dim to be parallel to. After you have created the first Ref Dim you can then
select this Ref Dim to orient the part for subsequent Ref Dims' creation.
Once you have your Ref Dims created, perform a Switch Symbols operation so
that you can see the Ref Dims' Symbol Names. Such as rd0 and rd1, as
examples only. You can also do this by choosing Tools - Relations.
2) Retrieve the generic model and choose Tools - Family Table. Click on the
icon for adding dimensions, features, etc. and choose the option named
'Other'. Pro/ENGINEER will prompt you to enter a Symbol Name. This is where
you can enter the rd0 and rd1 or whatever your Ref Dims Symbol Names turn
out to be after having created them in the flat state instance.
This should solve your problem. You can also use the 'Other' option to
include dimension tolerances in a Family Table. Not that there is much of a
demand for this type of thing, but I thought that I would offer that up to
you while I am discussing the 'Other' option in Family Tables.
Ron M.
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Wojtek
Guest
|
| Posted:
Fri May 06, 2005 4:01 pm Post subject:
Re: How to add driven dimension into the family table |
|
|
Thanks a lot for the information. It works, but not solves the main
problem. I've checked it doesn't work because Flat State became part of
a family table. You can add ref dimension into the family name, but they
are not updated when model is changed.
Anyway all the information I've received from you and from other guys is
extremely useful to try to solve the main problem by myself.
Seems ProE do not allow to create really useful family table for Flat
State in simple way. The only way is to create some parameters and
relations.
Wojtek
Ron M. wrote:
| Quote: | "Wojtek Weber" <wweber@gazeta.pl> wrote in message
news:d4q297$et1$1@inews.gazeta.pl...
I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
Thanks in advance.
Wojtek
WF1
You can test out the following technique to see if it provides you with what
you're looking for here.
1) Retrieve the flat state instance and add Part mode Reference Dimensions
to it. In Wildfire you can create Part or Assembly mode Reference Dimensions
two different ways. The first way is to choose Edit - Set Up - Ref Dim. You
will have to select a datum plane for the dimensions to be parallel to. The
second way is to add what is known as an Annotation feature Ref Dim in
Wildfire 1 or 2. There's an icon on your Wildfire toolbar for Annotations.
This approach also requires the user to select a datum plane for their Ref
Dim to be parallel to. After you have created the first Ref Dim you can then
select this Ref Dim to orient the part for subsequent Ref Dims' creation.
Once you have your Ref Dims created, perform a Switch Symbols operation so
that you can see the Ref Dims' Symbol Names. Such as rd0 and rd1, as
examples only. You can also do this by choosing Tools - Relations.
2) Retrieve the generic model and choose Tools - Family Table. Click on the
icon for adding dimensions, features, etc. and choose the option named
'Other'. Pro/ENGINEER will prompt you to enter a Symbol Name. This is where
you can enter the rd0 and rd1 or whatever your Ref Dims Symbol Names turn
out to be after having created them in the flat state instance.
This should solve your problem. You can also use the 'Other' option to
include dimension tolerances in a Family Table. Not that there is much of a
demand for this type of thing, but I thought that I would offer that up to
you while I am discussing the 'Other' option in Family Tables.
Ron M.
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