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I would start by making a feature that completely engulfs the one you want to remove, then copy&paste the radii surface that the feature is located on(this will be the surface you want to keep or be when finished, then you will use the feature edit>offset. This will replace your boss feature with the radii feature.
You can only have one surface replaced at a time tho.
here is your hole feature...........
this is the new feature engulfing the old one
this is the edit>offset feature..... using the copied surface to replace the feature.
tommy,
i created an extrude feature to cover the geometry i wanted to eliminate. however proe treats the model as a multibudy part now. how can i merge the extruded feature with the imported part so that i can use replace face tool? take a look at the part: (i trimmed the part to avoid the file being to big)
solidshill from Iran via Argentina via Chula Vista or wherever,
As the file version wasn't indicated I didn't bother downloading it,
but the basic procedure goes something like:
_Select the Import Feature, RMB -> Edit Definition.
_Menu: Geometry -> Heal Geometry -> Manual -> Edit Bndry
_Select a surf intersected by the features to be deleted.
_Delete Contour, cycle thru until the appropriate (hole) trim
boundary is highlighted and Accept.
_Repeat as necessary.
Once all the holes are closed either Delete (hit Delete key, then select
objects) the extra surfaces or put them on a layer and blank.
If that doesn't seem to fill the bill post something I can read in WF2
and I'll take a look at it.
And, please, do people the courtesy of trying to conjure an appropriate
subject line for the post.
can solidworks manipulated data like that within the imported file from Pro/E?Would SW recognize that IGES hole as a feature and remove it? Edited by: design-engine
Bart,
IGS data is completely flattened and SW does not recognize the part's features. feature recognition is possible but usually results in a confused history tree with a lot of useless features.it's more usefull for simple prismatic parts. i don't use that. it's easier to work with the dumb file as is.
i dont understand your first question what do you mean?
Well in a solieworks file that is imported into Pro/E... Pro/E iges functions can recognize the feature and delete it. Thats what Jeff is telling you in his post.
I smoked my work machine graphics card this morn, so can't look
at the neutral, but ...
> http://i33.tinypic.com/s4yrsm.jpg
... indicates you've deleted the trim boundary on the "body" radius
outside surf (good) but not on the radius inside surf (bad).
Starting fresh and putting it another way ...
Deleting the trim boundaries on both those surfaces where the boss
feature intersects the main body will orphan the boss, e.g. there's
no longer a main body edge there for it to join to so it will no longer
be a part of the main body. That, now discrete, quilt (set of surfaces,
shell, etc.) can then be deleted or hidden.
Terminology and verbal communication can get cumbersome but my usage of
most terms here is generic ...
"Feature" doesn't mean "program specific feature". When I say
"boss feature" it simply means the surfaces (fillet, tapered cylinder,
planar end cap, hole bore, c'bore, etc. surfaces) that represent the
tangible article feature.
"Body" doesn't mean Body in Parasolid or ACIS speak. It means, in this
context the quilt (also generically refered to as shell, where "shell"
is not a program feature) that represents the modeled object.
(There are also other ways to accomplish your intent; i.e. instead of
defining the import as a solid, define it as a quilt. You can then,
using standard model mode functions, use existing boundaries to trim away
unwanted geometry and copy existing surfaces using options to exclude
internal boundaries, etc. For this application I see no advantage, just
mentioning if you want to experiment.)
_ _ _ _
Bart,
Reading "Pro/E iges functions can recognize the feature" can lead to
a couple of gross misunderstandings ...
Pro/E does not have Feature Recognition functions (which doesn't bother
me a bit).
IGES doesn't have functions and beyond read / write routines Pro/E doesn't
have "IGES functions". It ~shouldn't~ matter at all if the translation is
done via IGES, STEP, ACIS, ParaSolid, etc. Geometry is geometry and the
definitions are standard. The differences, between "formats" or protocols
amount to no more than the way the established geometry structures are parsed
and stored in translation data structures. It's a pet peeve of mine; seeing,
especially common among Really (think ad$k)low end sales types, talk about
"IGES surfaces", how "they" are inferior or this or that; in some way
"special". IGES doesn't create or redefine surfaces, simply stores lists of
Control Vertices, Knots, attributes, transformation matrices, etc. written by
the source program. 99% of the time; when it doesn't work it's because of a
poor read / write implementation or incomplete geometry type support on the
part of the target program. Once a translation read is complete it's just
geometry again and there's no reason to differentiate what translation
protocol was used.
The problem is that your model is not a solid one to begin with. When I opened up your model it was in surfaces. You need to first close all your open surfaces and make your model solid before you can remove your feature.
follow the click sequence from my second post to get your model solid, then work at removing you feature.
tommy,
thank you. i followed your instructions and converted the closed surface into a solid with non-zero mass properties, but the extrude feature still adds another body to the part.(i tried extrude feature with a native part, and the result was a single body)
finally i played a little with modify command and found out that i could easily delete those unwanted surfaces.then removed the holes by deleting their edges and converted the closed surface into a solid.
jeff,
thank you. very informative post. you seem to have a good academic education on CAD plus wealth of experience.
now, how can i control the extrude feature or any other additive features to create additional body (create multibody part) or merge into the base part? (i searched "multibody","multi-body", "multi body" in the documentation and found no results
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i chopped it to get smaller)
