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assembly cut in a part drawing

donha

New member
While in the Assy, choose Feature/Intersect,choose thecut, choose the Level drop down and change it to "Part Level". Select the parts you want intersected at the part level.
 

burnsp

New member
donha - I did that and it didn't place the cut in the part drawing. I originally thought that was the answer also, but now I'm not sure what that drop down box does. If that does work, perhaps you can give me some more detail. Thanks.


dr_gallup - is this what you meant also?
 

dr_gallup

Moderator
Yes. Make sure it is intersecting the correct part and that the cut is applied at the part level. You may have to regen the assembly, the part & then the drawing view to get it to show up (depends on how you have config options set, something like "auto_regen_views").
 

donha

New member
You have to choose "View > Update > All Sheets" to make the changes appear to your drawing. This is true for almost any model changes made while the drawing is in session.
 

burnsp

New member
I did recreate the cut selecting 'part level' and it finally showed up in the part and the drawing of the part. Thanks for the help.
 

Heathbn

New member
FYI


Creating features in at the assembly level is always a bad idea. their are way to many reasons to list but the biggest is circular references.
 

jtma67

New member
I'm a relatively new user to Proe, but thought that creating parts in the assembly level is what "top down design" is all about...... wait a second... is creating a "feature" different than creating a "part" in the assembly level?
 

SRINIVASANIYER1

New member
Yes it is different.


You can create a part in assembly. You can also create a feature in assembly mode. Only take care that the part on which the feature is created is "ACTIVATED" before the feature is created. If the feature is unique to the part geometry in question, i.e no other part geometry reference is required, then it is always better to open the part and create the feature, lest you inadvertantly reference geometry of any other part.


Assembly cuts are useful in cases where you want the cut to appear in the assembly drawing but do not want it to appear in the part drawing. e.g being DOWELING an assembly with another, wherein the dowel hole is made in the assembly and not in the part. Another example could be FABRICATION and MACHINING.


Regards,
 

Heathbn

New member
You make parts in part mode and features in either part or assembly. However it is almost always a bad idea to make parts that are dependant on an assembly.


If you are just learning Pro-E you should avoid working in assembly mode as much as possible.


Example


If you have four plates that all have the same holes instead of using an assembly cut. Copy the feature location from a skel and make the cut in each part.
 

bsnath

New member
creating features in the assembly helps us, when this feature has to be referenced to an object which again has reference with another object in the assembly, whose location you are not sure about.
 

scubadude

New member
Maybe it's semantics, but I was taught, and agree with, that itis better to create the feature within the part and NOT the assembly. This is not to say, don't use the assembly references, etc. I think its better because you don't get accidental references to the whole assembly.


While in the assembly, you simply do a >modify>modify part>Feature>Create...


This allows you to create the feature you want using only the references you select. If you use the part's features to orient your sketch you can then select the other assembly references while in sketcher.
 

dr_gallup

Moderator
It is much easier to control references than it used to be. I think a lot of peoples phobias about creating part features in assembly mode comes from earlier releases of Pro/E where it was all too easy to inadvertantly create external references that would fail outside of the assembly. So I think it is OK to make part features in assembly if you are reasonably careful about what you reference and understand the implications.
 

Heathbn

New member
When you are designing anything more often then not it is more then one part. That being said the parts mean nothing by them self.


The whole goal is to have parts that fit together. However when you design something their is always more then one stage(assemble) that have some of the same parts. In order to continually move forward It is very important that Assemblies be completely throw away andnot referenced by the individual parts(as you work you never know if design 1,2,3 or 4 is going to be the final design).


If you want to share data from one part to the next you need to use a top down design (BIG picture first) approach. Its a lot like chessyou want to win while making as few moves as possible.


I order to do this you have to be able to watch the whole design all the time in many different possible configurations.


Tying your parts to your first configurations forspeed is always a bad idea.


In order to be able to reuse the data efficiently you have to make it robust and flexible to change of any type at any time in the process.
 

bsnath

New member
may be.


but while in the process of designing, the creating features in assembly helps a lot.we cant deny that and moreover it is not that bad to create features in assembly.as dr_gallop said, its the reference which matters.
 

Heathbn

New member
while I have stated many different reasons why you should not use assemble featuresyou have not stated a single reason why we should. How exactly does it help a lot and in what way does this benefit the design process.
 

bsnath

New member
consider this simple example.if you are designing an assembly of a repeated component, there is a component in the assembly which is having a profile changing from design to design. and there are components in the assembly which has reference to that component. in that kind of scenario if you use assembly feature , your design will be easy rather than changing the features for every design.


hope u got the idea.
 

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