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nico741-Visitor
1-Visitor
June 13, 2011
Solved

CWWARNING: ASSEMBLY CUT is entirely outside the model; model unchanged

  • June 13, 2011
  • 1 reply
  • 11044 views

Hi,

I have an assembly with a pattern assembly cut . The pattern of hole "cut material" of different part of the assembly.

As a result when I regenerate the warning "WARNING: ASSEMBLY CUT is entirely outside the model; model unchanged" is there any way to resolve this issue?

I want to keep the model made of different part to get the hatch and the line correct in the drawing. and I can't make the hole at the part level as it's at the junction of two plates.

Thanks for your help

Nicolas


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Best answer by Kevin

In this case you need to split the holes into two patterns to keep the message from appearing. The reason is as you described you have three parts in the list but the holes do not intersect all three parts. The message appears because for the first five holes they intersect two of the parts but for the third part in the list the holes "entirely outside of the model" since they don't intersect it. The same applies to the second five holes. One part is intersected the other two parts are not. If you're adding the parts manually to the list Automatic Update doesn't need to be checked. If you want, see what happens when you split the holes into two patterns. In each of the patterns only add the parts the holes intersect, for the first five there should be two parts in the list for the second five there should be one in the list. Otherwise, the warnings are going to continue to appear.

1 reply

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BrentDrysdale12-Amethyst
12-Amethyst
June 14, 2011

Hi Nicholas,

I am not sure that I understand your question but I am going to guess anyway.

I avoid assembly cuts and instead use Top Down Design with a Skeleton and Publish Geom/ Copy Geom to make sure different features, such as holes, line up in the assembly but to ensure that I have the the references well controlled. This method uses the AAX module which is in our Enterprise SE licences. This method means that all features other than those copyied across are in individual part models not as assembly features and you can trace where that information comes from.

Specifically I suspect that your patterned assmbly cut does have some aspects of feature creation (one or more) which are completely outside the model(s) and usually I treat any such warning as a remimder to do things more robustly (hence the TDD approach).

If you do not have the AAX to do the TDD method you can still use things such as a patterned axis in the assembly which you use as a reference in the parts or the much older and still robust Master Modelling method where you make your first part in your assembly the master model and you make datum features such as planes and axes plus surfaces e.g. a surface cylinder (extrude) as the hole reference. You layer everything off in the Master Model and just turn it on when you need to use it for references. You will need to ensure your use of information from other models is allowed. You will need to be very careful not to get uncontrolled cross references but it is good practice to be careful with these anyway.

Hope I have explained this well enough and that it helps at least a little bit.

Regards, Brent

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nico741-VisitorAuthor
1-Visitor
June 14, 2011

Hi Brent,

See the picture bellow . This is a welded fabrication I've added 10 holes at the bottom, 5 are cutting the pink and the gray part sand 5 are cutting the green part only.

Proe thinks the holes are outside the model? I can not add the hole in the individual part as multiple parts are cut and I would like to keep the welded fabrication as an assembly for drawing purposes.

Nicolas

assy_cut.jpg

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nico741-VisitorAuthor
1-Visitor
June 16, 2011

If the holes are made in one pattern the hole note in the drawing (3d note in the model) is made automatically and you can keep it parametric without having to create a variable to add all the pattern number.

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