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Reg: Pro-e Standard Format For Part

suganthan.mech
1-Visitor

Reg: Pro-e Standard Format For Part

Hello Buddies,

Are there any international format or standard for creating part in Pro/E? I mean thant modelling structure. Like in part profile hole, round and chamfer feature should come in last. I have worked in different type of companies. Every companyhasown model structures forPro/E part.Are they any standard modeling procedure is confirmed ny PTC?.

Kindly let me know

Suganthan Rajamanickam

Pro-e System Analyst

Trane Design Centre, India

Ingersoll Rand


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6 REPLIES 6

Suganthan,

Your structure looks fine. Many Pro-E uses place the rounds (fillets) &
chamfers at the end of the model tree. If using draft, the draft typically
comes before the round or chamfer feature.

I tend to group features and place the round at the end of the feature
group. In Pro-E, if a feature within a group fails (cannot be redefined),
this can cause the entire group to fail, so use this practice only if you
are sure the features are robust. Has the last version of Pro-E WF solved
this problem? In SolidWorks, folders are used in place of groups.

Attached is a document containing some suggested Pro-E modeling practices.
My actual practices may somewhat differ, but this is a good reference
document.

Chris

Chris,

Nice list and thanks for sharing. What's missing from many of the
suggestions is the why.

For example, "6) use HOLES when making holes..."

Really? I've missed the command that converts a round hole into a slot
or a hexagonal shape. The practice of using cuts allows placing and
dimensioning to construction lines to locate the cut, which means that I
can delete the round cut and replace it with any other cut I want and
never wonder what happened to the shown dimensions on the drawing. Hint
- they are still there. For the truly a-retentive, adding an axis point
that is used later as an assembly reference means that even the mating
fasteners won't notice the change. For those pressed into it - offset
the axis point so the mating fastener might be placed off-center in the
slot.

Many suggestions are good in context. Putting rounds late, and not
integral with sketches, is OK advice. But the main reason to do this is
so the stress analysts can suppress them without rebuilding the model.
Oddly, the advice does not mention that external rounds are what the
analysts are looking to be rid of and that fillet rounds often must be
retained so the analysis doesn't come back showing infinite stress
levels in the corners. Based on this look, all external rounds
could/should be one late feature, but fillets should be as
individualized as possible.

Dave S.

Chris Thompson wrote:
>
> Suganthan,
>
> Your structure looks fine. Many Pro-E uses place the rounds (fillets)
> & chamfers at the end of the model tree. If using draft, the draft
> typically comes before the round or chamfer feature.
>
> I tend to group features and place the round at the end of the feature
> group. In Pro-E, if a feature within a group fails (cannot be
> redefined), this can cause the entire group to fail, so use this
> practice only if you are sure the features are robust. Has the last
> version of Pro-E WF solved this problem? In SolidWorks, folders are
> used in place of groups.
>
> Attached is a document containing some suggested Pro-E modeling
> practices. My actual practices may somewhat differ, but this is a good
> reference document.
>
> Chris
>

Dave,



I did not write the list. I had received it a few years ago from another
Pro-E user as indicated by the author and company name, so that is why I
mentioned my actual practices differ somewhat from the list. If someone has
a updated list of best practices, please send it.



You are correct about the stress analysis. I do not have Pro/Mechanica, so I
do not typically worry about stress analysis with Pro-E parts. However, my
license of SolidWorks does include simulation (static FEA), so I create a
separate configuration (Pro-E family table equivalent) with the rounds /
fillets, draft, and chamfer features suppressed. I leave the round
unsuppressed if it is critical to the analysis (ex: intersection of
cantilever beam attached to wall). Use of symmetry (cutting part in half) is
also recommended for FEA.



If it is a thin part, I use shell mesh by creating a mid-surface and
removing the solid body (automatically done with sheet metal parts). This is
really outside the original scope of the discussion, but it is important to
consider with modeling for both manufacturing and FEA.



Concerning the "6) use HOLES when making holes... ", I have done it using
both methods. If I anticipate the hole may become a slot, I model the
feature as a cut as per your suggestion. If I know that only the hole size
will change, I prefer to use holes especially if the hole have receive a
c'sink or a c'bore. The same of threaded holes. I am guessing this is what
the author had in mind as well.



Anyway, If anyone has a improved list, or better a CAD neutral list (Pro-E,
SolidWorks, etc.) of best modeling practices, feel free to share it. These
practices may also differ somewhat between the person modeling for CAD / CAM
in a machine shop versus the design engineer at a company that does not
manufacture in-house.



Chris


With regard to using HOLES to make holes, in addition to what Chris has
said, using holes will allow you to create hole tables in a drawing.
When the hole feature is a cut, it will not be picked up by the hole
table



Robert

I find occasional review of these types of lists refreshing. As
previous lists have been posted to the group, I've combined them in a
google doc:



Hello Chris,

Thanks for your valuable reply. Sorry for the dealyed reply from my side. Your attachment sounds great. I have try to create standard practice method for modeling and assembly. Thats why want to know that any international standard available for part modelling. So now we have confirmed that did not exist. So I will create it for my company. If i get any documents I will send to you.

Keep in touch

Suganthan Rajamanickam

Pro-e System Analyst

Trane Design Centre, India

Ingersoll Rand

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