Here is a work around for your problem. I am not sure how robust this
is but I tried few things quickly and came up with this.
(I am referring to your picture)
Before deleting the first cut, try to follow these steps
Show Hidden for the part since all the Ref geom is hidden.
The order for the reference geometry in the history tree will be Rf
Plane, Rf Point, Rf Line
Modify the reference point for second cut, move associations.
Pick the reference point for the first cut,
pop up form will ask you to pick the feature you want to move, pick
pattern and hit OK
update the part
try suppressing/deleting the first cut and then changing the dim for
the coordinate system
see the attached gif
Hope this helps.
Good luck
Randy,
Does it make any difference if you manually create ref
lines/points/planes
on top of the coord systems, rather than letting Ideas do it
automatically?
(On re-reading this email, I suspect that may be what you meant by
creating
"junk" ref geometry).
It always bugs me that it hides the "automatic" ones, since they then
aren't
visible for picking the next time I want to use them.
I haven't checked this, but does it create new ref geometry if you just
pick
the co-ord system again, or is it clever enough to know that it already
created some over the top of the CS?
My other thoughts are:-
a) Why the hell can't it use the CS directly for these operations?
After all, it manages to use them for assembly constraints.
b) Why are we stuck having to use cutter parts at all, to create tapped
holes???
> Alan,
> A co-worker of mine has called it in and has been working a bunch
with the
> hotline. They have confirmed that it is a serious problem, and is
looking
> into when a fix can be implemented (PTF, m-release, I10).
>
> Until that happens we are looking into possible work-arounds within
our
> company. Since we do a lot of cut with relations this is already
affecting
> us. Here's what we are looking at.
>
> -This only affects parts that were created in I9
> -This only happens when the feature before the cut is deleted. Could
> suppress it instead.
> -One work-around is to locate the cut from reference planes, points
or
> lines. No additional reference geometry is created when you use
something
> other that coord systems. Why, I don't know! I don't prefer this
method.
> -I think the best work-around is what the hotline suggested. Create
some
> kind or junk reference geometry before every Cut operation you
perform.
> That way a separate node gets created before each cut that will not
get
> deleted. We are looking into creating a global symbol that will
first
> create a ref point, then hide it, then execute the Cut command. That
way
> all the users have to remember is use a global symbol instead of the
actual
> Cut command. The history tree will get slightly larger though.
>
> Haven't got any reasoning behind whats happening, the only thing I
can
think
> of is they changed the location/owner of the ref geometry that gets
created
> when you do the Cut.
>
> I'll pass along any additional information I may get.
> Randy Stucke
> Minster Machine Co.
> Minster, OH
Milind
-----Original Message-----
From: Randy Stucke [mailto:StuckeR@MINSTER.com]
Sent: Tuesday, February 11, 2003 3:20 PM
To: iccon-des@loki.sdrc.com
Subject: [iccon-des] I9 Cut/Coord system problems
Icconers,
We are seeing a disturbing thing happening (loss of associativity) with
coordinate systems in I9m2 and wanted to see if anyone else is seeing
this
too.
We always start a part with a BORN and very often use additional
coordinate
systems to locate other key areas of our parts that many cuts and
extrudes
will be located off of (for design intent reasons). The problem we are
seeing is happening when we do a "Cut with Relations" and locating it
relative to any additional coordinate systems.
Here's an example of what we are seeing, see attached pics.
-Created a BORN
-Created an additional coordinate system (yellow one) translated from
BORN
-Sketched on xy plane of BORN and extruded a square to create Join5.
-Created the blue patterned cutter part (our method of creating tapped
holes)
-Cut with relations and dimension it from the second (yellow) cord
system
axis. We typically use the "from edges" and "parallel edges"
positioning
commands for our cuts.
-Created the orange patterned cutter part.
-Cut with relations and dimension it from the second (yellow) cord
system
axis too.
Because I located my "cut with relations" from the coordinate system it
created three additional pieces of reference geometry on top of the
coord
system for each Cut that will control the location. It also placed them
before each of the cuts (see history tree). Apparently it created
these
extra pieces of ref geometry in previous releases but placed them in a
different location.
Every thing is ok at this point, if I change the location of the
second
coord system, the two cuts will keep its relationship according to it,
which
is what we want.
Now, if I decide to delete the first Cut (Pattern 9) from the part, it
gives
me a warning that it is also going to change the 3 pieces of reference
geometry for the second cut to Key-In, thus making my second cut not
located in relation to the second coord system anymore. If I then
modify the
coord system location, the second cut will not update its location.
Now I have to go and delete then re-add my relations for the second cut
if I
want them to keep the correct design intent. Thats great.
Anyone else seeing this? Have any bright ideas to fix this.
Seems like one more great enhancement that broke something else.
thanks,
Randy Stucke
Minster Machine Co.
Minster, Ohio作者: zlz1976 时间: 2003-2-13 15:13
Assembly meshing
Darryl,
Partition Join is available in Ideas9, under the
Cut/Join/Intersect icon stack. In Ideas8 you can find it
as a hidden command /xto/co/pj. Veyr useful for us
analysts!
regards
---- original message ----
>Manoj,
>When creating meshes on an assembly consisting of
>multiple parts, and with varying material properties,
>I prefer to create a single I-deas part. My procedure
>is to either partition the part into volumes representing
>each actual part, or more preferably take advantage of
>the new feature to "Replace Operation" to "Join
Partition".
>
>For basic partitioning, simple sketch-in-place one
>or more non-intersecting lines and select "artition"
>for the operation. However, I have seen many cases
>in which the partition operation fails, should the
>desired interface be somewhat complex, i.e. given
>a solid plate onto which a set of flanges has been
>extruded in a cross-hatched fashion. The operation
>"may" fail when attempting to partition off the
>set of flanges into a single volume (to assign a
>different material property). Also, the partition
>operation adds another feature in the history tree.
>
>Nowadays, I prefer to first Join the new feature to
>the base part, and then ctrl-m, Modify, Special
Techniques,
>Replace Operation, Join Partition, [select feature].
>This creates a partitioning surface where the new
>feature is joined. One can Join Partition newly
>created features as you go, or create all the features
>and Replace Operation, Join Partition afterwards.
>The method works for complex volume interfaces.
>
>With this approach, I have created complex assemblies
>as a single part, yet with a large number of volumes
>with complex interfaces between the volumes. This
>allows convenient assignment of material properties
>to the mesh associated with each volume, and
conforming
>meshes at the interfaces. Naturally, this approach
>assumes tight connections at the volume interfaces.
>
>erhaps I-DEAS 10 will take this one step further
>and allow one to select Join Partition during the
>initial join operation. I requested this enhancement
>via IR Number: 4660555
>
>Darryl Chong
>IBM Storage Systems
>San Jose, CA
>
>--- "McDougal, Alan" <Alan.McDougal@goodrich.com>
wrote:
>> I do about the same thing you do but I use
associative copy to bring all
>> the
>> volumes together. I come from a design
background so I'm pretty
>> comfortable
>> with AC. If you're not comfortable with it, it can be a
hard path to
>> follow. The upside is it makes everything much
more associative and, I
>> think, easier to manage for geometry changes. I
then use groups to work
>> with individual volumes.
>>
>> Unlike you however I usually model things to mean
condition and let the
>> interfaces fall where they may. I generally do
contact from there. The
>> main thing to be aware of here is that if you have
overlapping or "just
>> touch" volumes, you will need to do all you're cuts
and partitions in the
>> branches of the tree and not after the volumes have
been added.
>>
>> Alan McDougal I9m1
>> Structures Engineer HP-Unix v11.0
>>
>> Goodrich
>> e-mail: alan.mcdougal@goodrich.com
>> phone: (937)440-2031
>> fax: (937)440-3639
>>
>>
>>
>> -----Original Message-----
>> From: Dunlap [mailto:hznd58@atd.gmeds.com]
>> Sent: Tuesday, January 28, 2003 11:04 AM
>> To: keshavan@us.ibm.com
>> Cc: iccon-sim@loki.sdrc.com
>> Subject: [iccon-sim] Re: Assembly Meshing
>>
>>
>> Manoj wrote:
>>
>> >> I would like to know based on the experiences of
users what technique
>> >> they find the most convenient while building an
FE model of a complex
>> >> part.
>> >>
>> >> Specifically,
>> >>
>> >> 1.) When I build FE models of individual parts
and combine them, the
>> >> meshes are never completely aligned since the
part geometry is
>> >> complex. Hence I find myself moving nodes
around a lot. Since IDEAS
>> >> does not allow having more than one FE model
on the workbench, I can
>> >> not project the nodes from one model to the
next which would have
>> >> saved me a lot of time and trouble in meshing
>> >>
>> >> 2.) What I have been doing instead is combine
all the parts into one
>> >> giant part and create an FE model of that.
However I don't have much
>> >> control over the mesh this way.
>> >>
>> >> Is there a better way to do align meshes?
>>
>>
>> The developers of I-DEAS have made at least three
attempts to work towards
>> analyzing "systems" of multiple parts. They realize
they still have more
>> work
>> ahead of them and getting it right would be a
functional differentiater in
>> attracting new customers.
>>
>> That said, the approach I use is to "add" all the
parts into one master
>> part/Fem, leaving small gaps (say 1 mm) at the
part interfaces. I then
>> generally use the split surface command to create
matching surface
>> topography
>> and use the dependent surface command to get the
surface meshes identical
>> when
>> mesh all of the solids. I then use coupled_dofs
to "glue" the nodes at the
>>
>> interfaces together. Basically everything except for
the coupled_DOFs is
>> history supported so modifications are easy to do.
The reason for leaving
>> a
>>
>> small gap between the parts is just for convenience
so you are not working
>> with
>> coincident surfaces/nodes which makes graphical
picking more difficult.
>> Using
>> coupled_DOF's also allows you to recover the
interface forces if you are
>> looking
>> at load sharing across a complex interface (i.e.,
multiple bolts).
>>
>> Keith Dunlap
>> Allison Transmission
>> General Motors作者: zlz1976 时间: 2003-2-13 15:20
Node Selection
Manoj,
When prompted for the node to which you want to attach the spring, pick
RMB
Related To, then pick the anchor node.
If there are no nodes yet, you'll have to use geometry-based other
elements,
as described below:
---To do this, your anchor nodes must be on an edge or surface. Before
creating your anchor nodes, create reference points where you'll want
the
anchor nodes. You must create the reference points using the RMB On
Surface
or RMB On Edge options.
---At this point you could define anchor nodes on the reference points
you
just created, but it's not necessary.
---Pick the Define Other Elements icon, and from its subpanel pick
Define a
spring between two points. You're prompted to pick centerpoints, ref
points, vertices, edges or surfaces. You can pick the reference points
and
the element will be defined.
---If you used anchor nodes above, then instead of picking the ref
points,
you could pick RMB Between Anchor Nodes, pick the anchor nodes, then
when
prompted pick the geometry associated with the anchor nodes/ref points,
and
key in a position tolerance. I-DEAS will search around for ref points
close
to the anchor nodes and define the springs between those ref points
(thus
it's kind of redundant to have the anchor nodes).
---Now generate your solid mesh (the spring element definitions will
force
creation of nodes at the ref points even if you don't have anchor
nodes).
---Then generate other elements, and the springs will appear, attached
to
the reference points.
I don't generally use assembly FEMs and I know there are at least 4
ways of
doing it:
---join/partition all the parts then mesh as a whole with connections
---add all the parts then mesh each volume and connect them together
(or
append the FEMs, which does the same thing but without parts)
---Assembly FEM, which automates the previous option
---FEM From Assembly, which uses the assembly instances/configurations
to
place appended FEMs
I use the first method almost exclusively, and either way of picking
spring
points would work with this method. If you're using one of the methods
where you've already got meshed parts, then you should be able to use
the
first way of picking spring points. Since I never use Assembly FEM or
FEM
From Assembly, I don't know how my picking methods would work.
I hope at least some of this helps you with your problem!
Andy Wells
Sr. Mechanical Engineer
Electro Scientific Industries
Portland, OR
wellsa@esi.com
I've an assembly FEM created (consisting of a number of FEMs). I'm now
trying to connect them. I've defined anchor nodes (saved in groups)
for
each of the individual FEMs where they are to be connected (say using
springs). However, IDEAS does not allow me to define springs between
two
anchor nodes. It will only define a spring between nodes. However,
this
defeats the very reason I used anchor nodes to start with. How do I
retrieve the nodes that correspond to the anchor nodes?作者: wolfzcg 时间: 2003-2-15 08:04
:-e
artition"