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Hello All,
example: I've two solids in assembly mode and make straight hole through all of them.I need to get updated solids ( with hole now) in part mode.
Intersect option doesn't work - what is proper solution in cases like this?
Intersect parts with assembly cuts have never been brilliant in Pro/ENGINEER. There is the option to change the cut to 'part level' but I have never been able to get this to work. In actual fact, Pro/ENGINEER makes new parts in session (called something like AF0$$$$$$) and puts the assembly cuts onto these parts, so the cut you are seeing isn't actually cutting material in the assembly but at the part level and making it look like the cut has been created at the assembly level, even though it shows in the model tree. If you do want to make the cuts in your parts, then I would suggest making one of your parts 'active' in the assembly, making a cut which uses references from your assembly and then this will be shown at the part level. You can make other parts become 'active' to perform the same operation on them, using the original cut as a reference if need be. Cuts in assemblies have never been overly stable with regards to how 'automatic intersect' works because often it can lose reference to parts and the workaround sometimes is to change it to manual and physically add the parts you want intersecting.
generaly grzegorz you must first have a clear idea of the func of cut tool in assembly
it works in the same as in real life when you have a two plates and you drill them to have holes in the exact position, so before you assembled them you have no holes, right?
so the same in pro\e - you can not have a hole\cut in model if You made it in assembly, because your original part is without that
this funcionality many firms use to create machined parts - the orignal rough part is assembled in empty assembly, all you can do is make only cuts, just like in real world when you machine a part
so if you need to have a cut made in assembly and in part, you have to make this volume as another part and than use Edit>Component operations> cut out
If you are 'machining' a part from a casting then the best method is to mege the original into another parts and create all your cuts this way. Casting changes will be reflected in the machined part.
My knowledge may be out of date but I remember at one time assembly cuts were written into each affected part in the form of a "hidden instance" which is default.
This is the AF0## part mentioned earlier and it's actually an instance not a part. There may be a config option to change this in some manner, try searching on "hidden instance".
If you need to see the hole then you could always "modify part" in assembly mode and copy the hole features into it that way. Or "copy geom".
The mark of the best modellers is they try to mimicreal life as closely as possible intheir modelingnot only geometry wise but process wise too. Edited by: dougr
to be precise - i would better use copy geom than merge because with merge you copy all stuff that could be not necessary in machined part like quilts which not made a solod geaom, reference datums, axis, curves, all layers, cosmetic etc
but what is better - merge or copy geom? I suppose it a topic for another thread
"Intersect parts with assembly cuts have never been brilliant in Pro/ENGINEER."
My experience has shown that it's usually not Pro/E that's the issue, it's the help documentation and the lack of experience of the people writing it and supporting it who don't know the software.
In Solidworks assembly features are termed "time dependent features" andare very limited in comparsion to Pro/E...
How the term "time dependent features" relates to their real fuctionality is beyond the walnut size brain of this user.
Merge is far superior. Don't worry about quilts, datums, points, curves... just hide the merge in the model tree > save status in layer tree and all non-solid geometry will be hidden permanently. You can still use datum references which have been hidden if you unhide to select.
"Intersect parts with assembly cuts have never been brilliant in Pro/ENGINEER"
Try using silhouette edges for assembly reference cuts in a generic with family table instances which intersect a few parts. You will end up going round in circles with missing references in the instances. Redefining in the instance will only cause the generic to fail and vice-versa. PTC know about it but don't understand why it does it. This issue went right to the top of technical support at PTC a few years ago.
Hey grz, its seems to me that pjw got it right thare in his last post. Assembly level features are all well and good, but to be honest, in the many machines that I have designed I find that creating a hole in the first plate (its up to you which one you start with) and then add in thesecond parts holesusing the first hole from the first part as a sketch reference. When I add many holes I add then in as extruded cuts intially as it is much easier when designing than using the hole feature.
Let us know how you get on and what you did to get around the problem.
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