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copying bodies 2
- Thread starter skanskan
- Start date
JohnRBaker
Mechanical
What version of NX are you using?
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
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1
- #3
JohnRBaker
Mechanical
It really doesn't make any difference if you're using anything back to NX 6.0 or so, just that some of the terms you used were odd.
OK, you mentioned three methods for making a copy of a body (there are actually some others but we'll not confuse you with those for now).
Anyway, to the questions you've asked, I assume that the first two pertain to...
Insert -> Associative Copy -> Extract Geometry...
...where you've selected the 'Body' type. If you toggled ON the 'Associative' option in the settings section but NOT the 'Fix at Current Timestamp', the copy will always end-up as the LAST feature in the Part Naviagtor. In other words, once 'extracted' it will continue to update whenever features are added or modified. If you had also toggled ON the 'Fix at Current Timestamp' then the body that is extracted will NOT move when new features are ADDED to the model but it would update if any of the feature created before the 'extraction' were modified. Now if the 'Associative' option is toggled OFF, then by default it will be created at the current timestamp and it will not move when new feature are added the original model, and it will NOT update if older features are modified.
As for the Move Body using the 'Copy' option that works sort of like Extract without using the 'Associative' option. The only re difference is that you get to move the copy whereas in the Extract function the copy ends-up being the same place as the original.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
OK, you mentioned three methods for making a copy of a body (there are actually some others but we'll not confuse you with those for now).
Anyway, to the questions you've asked, I assume that the first two pertain to...
Insert -> Associative Copy -> Extract Geometry...
...where you've selected the 'Body' type. If you toggled ON the 'Associative' option in the settings section but NOT the 'Fix at Current Timestamp', the copy will always end-up as the LAST feature in the Part Naviagtor. In other words, once 'extracted' it will continue to update whenever features are added or modified. If you had also toggled ON the 'Fix at Current Timestamp' then the body that is extracted will NOT move when new features are ADDED to the model but it would update if any of the feature created before the 'extraction' were modified. Now if the 'Associative' option is toggled OFF, then by default it will be created at the current timestamp and it will not move when new feature are added the original model, and it will NOT update if older features are modified.
As for the Move Body using the 'Copy' option that works sort of like Extract without using the 'Associative' option. The only re difference is that you get to move the copy whereas in the Extract function the copy ends-up being the same place as the original.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #5
Maybe just one additional explanation for 'Extract body here' option.
This is not part of the Extract Geometry command. When you use Extract Geometry command, it will be created as the last feature in the Part Navigator. And according to the 'Fix At Current Timestamp' it will behave as JohnRBarker already explained.
Now, if you have already created your model and want to extract body in let's say step 3 of finished model, there is another story. With Extract Geometry, you would have to make this step3 as current feature and then use this command. But, with Nx8 (and later), you can do the following:
1. click with right mouse button on the step3 in part navigator.
2. from the menu, select 'Extract body here'
3. at this point in part navigator, the new body will be extracted. Just as if you would make this step current feature and then use Extract Geometry command.
So, the difference between 'Extract body here' and 'Extract Geometry' is, that the first one will save you clicks and time, when you have to extract the body in a specific timestamp of already created model.
I hope, that this explanation is clear enough.
This is not part of the Extract Geometry command. When you use Extract Geometry command, it will be created as the last feature in the Part Navigator. And according to the 'Fix At Current Timestamp' it will behave as JohnRBarker already explained.
Now, if you have already created your model and want to extract body in let's say step 3 of finished model, there is another story. With Extract Geometry, you would have to make this step3 as current feature and then use this command. But, with Nx8 (and later), you can do the following:
1. click with right mouse button on the step3 in part navigator.
2. from the menu, select 'Extract body here'
3. at this point in part navigator, the new body will be extracted. Just as if you would make this step current feature and then use Extract Geometry command.
So, the difference between 'Extract body here' and 'Extract Geometry' is, that the first one will save you clicks and time, when you have to extract the body in a specific timestamp of already created model.
I hope, that this explanation is clear enough.
Shadowspawn
Aerospace
Skanskan... Instance Geometry is another method... which I think will be replaced w/a flavor of 'patterning' at some point.
Regards,
SS
CAD should pay for itself, shouldn't it?
Regards,
SS
CAD should pay for itself, shouldn't it?
JohnRBaker
Mechanical
'Instance Geometry' has been replaced with 'Pattern Geometry' in NX 9.0. In fact, in NX 9.0 we've pretty much replaced all the 'make copies of things' functions with a series of 'Patterning' functions which all share a common 'look & feel' as well as many similar 'Patterning schemes'. In addition to the Sketcher 'Pattern Curve' function (introduced in NX 7.5) and 'Pattern Feature' (introduced in NX 8.0), we now have 'Pattern Geometry', 'Pattern Face' and 'Pattern Component'.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #9
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1
- #10
JohnRBaker
Mechanical
Well, lets say you've got a design where there are some variations and you'd rather just have two (or more) models instead of turning a bunch of features ON and OFF to represent the variations. What you could do is create the model up to the point where all the features are common to the variations. Then you do an Extract Body using the 'Fix at Current Timestamp' option so that you now have two identical models that from there you can add the unique features to either or both models (of course you'll probably have to do some selective Hiding and Showing to get access that only one model at a time but I'll explain how that can be easily done later on). Now when you've finished you'll have models which if you edit the features which were created before the Extract Body feature, it will cause BOTH models to update, whereas editing features created AFTER the Extract Body operation, they will only update their respective models.
Now you can get very creative if you wish, as I've already alluded to earlier, where you could have several different variations and the Extractions could have been performed at various points along the 'history' of the model so that you could have different levels of 'common features' for each variation. Now it's critical that you have to use the option where these extractions are defined as being 'Fixed at Current Timestamp'. Once you've got what you want you can assign each variations to its own Reference Set so that when this model is added to an Assembly you can pick and choose which variation that you want to use, and since ALL of these variations are collocated in the same place and orientation in the master model, even if the Components in the Assembly were not constrained, you could replace one variation with another and there would be no chance that they would move or be oriented differently.
Now this does bring up something that people may have been wondered about.
Have you ever looked at the Part Navigator and wonder why there's a 'Timestamp Order', or to be more exact, why would you want to toggle 'Timestamp Order' OFF? Well this is one of those situations where this is handy, when there are MORE THAN ONE model in the same part file, which would be the case if you were doing what I described above. When you're not in the 'Timestamp Order' mode you'll be able to see all the variations and by looking at how the features are related to which body you can get a better understanding of how all the variations were created. Also, while you've in this mode, it's very easy to toggle the display of the various 'models' ON and OFF (Show and Hide) which makes it very east to go back and forth to work on the variations, as shown below:
Anyway, I hope that helps to explain one the primary reasons why NX has this capability of Extracting Bodies yet leaving them collocated.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
Now you can get very creative if you wish, as I've already alluded to earlier, where you could have several different variations and the Extractions could have been performed at various points along the 'history' of the model so that you could have different levels of 'common features' for each variation. Now it's critical that you have to use the option where these extractions are defined as being 'Fixed at Current Timestamp'. Once you've got what you want you can assign each variations to its own Reference Set so that when this model is added to an Assembly you can pick and choose which variation that you want to use, and since ALL of these variations are collocated in the same place and orientation in the master model, even if the Components in the Assembly were not constrained, you could replace one variation with another and there would be no chance that they would move or be oriented differently.
Now this does bring up something that people may have been wondered about.
Have you ever looked at the Part Navigator and wonder why there's a 'Timestamp Order', or to be more exact, why would you want to toggle 'Timestamp Order' OFF? Well this is one of those situations where this is handy, when there are MORE THAN ONE model in the same part file, which would be the case if you were doing what I described above. When you're not in the 'Timestamp Order' mode you'll be able to see all the variations and by looking at how the features are related to which body you can get a better understanding of how all the variations were created. Also, while you've in this mode, it's very easy to toggle the display of the various 'models' ON and OFF (Show and Hide) which makes it very east to go back and forth to work on the variations, as shown below:
Anyway, I hope that helps to explain one the primary reasons why NX has this capability of Extracting Bodies yet leaving them collocated.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
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- #11
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