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NX9 Blending Instances
- Thread starter pzang
- Start date
JohnRBaker
Mechanical
Note that this change actually took place with NX 8.0 when we introduced Pattern Feature, but it works the same in NX 9.0 as it did in NX 8.0/8.5.
First off, the 'capability' is still there, just that explicit 'Blend/Chamfer All Instances' functions are no longer needed.
In fact, you actually now have two different approaches that will work for you, so you can pick the one that will be best suited for the way you like to work. But first a little history lesson; the reason that we even NEEDED the 'Blend/Chamfer Instance' function in the past was because we did NOT allow you to include Blend or Chamfer features as part of the Instance itself, they had to added AFTER the Instance was created, thus the need for some automated 'function' and so was born the 'Blend All Instances' and 'Chamfer All Instances' options added the the respective Blend and Chamfer dialogs. Now you can add your Blend/Chamfer to the feature and simply include them when you select your feature to Pattern. What could be more straight forward than that?
Now the second approach does more closely follow the older workflow and besides, if you're the type who prefers to add details like Blends and Chamfers near the end of the model tree then go ahead work like you've done before, creating your Patterns without any Blends and Chamfers and then when you're ready to add the Blends/Chamfers, simply add a single Blend/Chamfer feature to ANY member of the Pattern of interest and using the Pattern Feature function, only this time selecting just the Blend/Chamfer feature, then in the 'Pattern Definition' section of the dialog set the 'Layout' type to 'Reference', then select any one of the Pattern's features, thus selecting the Pattern, and then you will be asked to select the 'Handle' of the feature that will be the 'base instance' for this NEW Pattern which is almost always the handle for the original Pattern's feature that the Blend/Chamfer was added to. Now hit OK and you'll have done, in essence, a 'Blend/Chamfer All Instances' operation. Granted, the model tree will look a bit different, but the order of updating will be basically the same as if was using the old pre-NX 8.0 workflow.
Anyway, I hope this was what you're looking for.
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.
First off, the 'capability' is still there, just that explicit 'Blend/Chamfer All Instances' functions are no longer needed.
In fact, you actually now have two different approaches that will work for you, so you can pick the one that will be best suited for the way you like to work. But first a little history lesson; the reason that we even NEEDED the 'Blend/Chamfer Instance' function in the past was because we did NOT allow you to include Blend or Chamfer features as part of the Instance itself, they had to added AFTER the Instance was created, thus the need for some automated 'function' and so was born the 'Blend All Instances' and 'Chamfer All Instances' options added the the respective Blend and Chamfer dialogs. Now you can add your Blend/Chamfer to the feature and simply include them when you select your feature to Pattern. What could be more straight forward than that?
Now the second approach does more closely follow the older workflow and besides, if you're the type who prefers to add details like Blends and Chamfers near the end of the model tree then go ahead work like you've done before, creating your Patterns without any Blends and Chamfers and then when you're ready to add the Blends/Chamfers, simply add a single Blend/Chamfer feature to ANY member of the Pattern of interest and using the Pattern Feature function, only this time selecting just the Blend/Chamfer feature, then in the 'Pattern Definition' section of the dialog set the 'Layout' type to 'Reference', then select any one of the Pattern's features, thus selecting the Pattern, and then you will be asked to select the 'Handle' of the feature that will be the 'base instance' for this NEW Pattern which is almost always the handle for the original Pattern's feature that the Blend/Chamfer was added to. Now hit OK and you'll have done, in essence, a 'Blend/Chamfer All Instances' operation. Granted, the model tree will look a bit different, but the order of updating will be basically the same as if was using the old pre-NX 8.0 workflow.
Anyway, I hope this was what you're looking for.
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
- #3
Hi John,
I wondered about this when creating the attached part, in which you can't include an outer blend in the original pattern because it affects adjacent instances.
So I've just followed instructions for pattern feature, select blend, reference original pattern, select handle and so on, and the instance locations do look like the blends will appear in the correct locations, but then I get an error (parent failed to update).
If you have chance, could you see if I'm missing something? Thanks.
I'll upload some pictures too because I did this one in NX9.
NX 7.5 with TC 8.3
I wondered about this when creating the attached part, in which you can't include an outer blend in the original pattern because it affects adjacent instances.
So I've just followed instructions for pattern feature, select blend, reference original pattern, select handle and so on, and the instance locations do look like the blends will appear in the correct locations, but then I get an error (parent failed to update).
If you have chance, could you see if I'm missing something? Thanks.
I'll upload some pictures too because I did this one in NX9.
NX 7.5 with TC 8.3
JohnRBaker
Mechanical
I'll take a look and let you know what I discover.
BTW, as you've noticed, you can only upload a single file at one time, so it's best in a situation like this one to first zip the 3 files together and then upload that file.
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.
BTW, as you've noticed, you can only upload a single file at one time, so it's best in a situation like this one to first zip the 3 files together and then upload that file.
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.
Thanks John, and tip noted... yes I did feel foolish posting 3 times!
NX 7.5 with TC 8.3
NX 7.5 with TC 8.3
JohnRBaker
Mechanical
What you've run into is one of the those cases where there is nothing that can be properly referenced for this to work since the original pattern doesn't actually include the edge that the blend is referencing, it's being created by the Boolean feature. It's a sort of 'Catch-22'. However, I did come up with a solution to your problem (of getting all the 'teeth' belended in on eoepration) which did not involve using a second Pattern. Now this might not work so well if your goal was to make a 'sprocket' which will be 100% parametric in that you could edit the number of 'teeth' (however, if you edit it to have LESS 'teeth' it just might).
What I did (see attached example) was to simply go into Blend edge, set my size, rotate the model around so that I was looking at the 'sprocket' from the side... heck, it'll be easier to just watch the included video to see what I did. Don't worry about those tangent edges at the bottom of the 'teeth' as NX will simply ignore them when it creates the blends, but of course you do need to deseelct those two edges inside the 'bore'.
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.
What I did (see attached example) was to simply go into Blend edge, set my size, rotate the model around so that I was looking at the 'sprocket' from the side... heck, it'll be easier to just watch the included video to see what I did. Don't worry about those tangent edges at the bottom of the 'teeth' as NX will simply ignore them when it creates the blends, but of course you do need to deseelct those two edges inside the 'bore'.
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.
Here is also mine example. I have edited the sketch so that the blend/fillet is already in the sketch. There is little bit more work to do, but this can be one possible solution. But for this particular example, John has given much more simple solution.
Anyway, I hope that this example Will help, too.
Regards.
Anyway, I hope that this example Will help, too.
Regards.
Thank you Sven and John, two different that can work.
It's an interesting one because it does actually work with the old "blend all instances" option after an array. Have been looking at this as part of a training project, so I'll just come up with a different way of doing it.
Thanks for your help, Carl
NX 7.5 with TC 8.3
It's an interesting one because it does actually work with the old "blend all instances" option after an array. Have been looking at this as part of a training project, so I'll just come up with a different way of doing it.
Thanks for your help, Carl
NX 7.5 with TC 8.3
- Thread starter
- #12
Ok John,
Another challenge, same topic. I am creating the blends on the end of the IMPELLER of the impeller (CAST) assembly. I cannot figure out a way to include the blends to all of the blades I create (6) without the "blend all instances" command? I have attached the Bottom and Top Housing along with the Impeller with one blade.
Another challenge, same topic. I am creating the blends on the end of the IMPELLER of the impeller (CAST) assembly. I cannot figure out a way to include the blends to all of the blades I create (6) without the "blend all instances" command? I have attached the Bottom and Top Housing along with the Impeller with one blade.
JohnRBaker
Mechanical
This is one of those cases where 'Pattern Face' proved to be a better solution (see attached 'Impeller' file).
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.
Another option here is to not unite the extrude (fin) feature with the central cone.
So, you can trim and blend the fin only, then unite, and then use the pattern feature command.
The problem you have is that your trim affects a solid created by the cone and fin joined together (as the model is at the moment).
At least I think that's right!
NX 7.5 with TC 8.3
So, you can trim and blend the fin only, then unite, and then use the pattern feature command.
The problem you have is that your trim affects a solid created by the cone and fin joined together (as the model is at the moment).
At least I think that's right!
NX 7.5 with TC 8.3
JohnRBaker
Mechanical
While what Carl suggested would mitigate the issues a bit, there's still the sheet body used to trim the impeller which will still cause some issues. As I stated, this is a classic example of why we've implemented the 'Pattern Face' function. And while, if we had not had these 'linked' secondary bodies issue, we could have used Pattern Feature, I would still opt for the Pattern Face since the result would be a smaller model that updated faster with a cleaner feature tree and besides, unlike some other situations, it's highly unlikely that you have ever needed to use the ability to edit ONE of the 'instanced' features making it different from the other impeller blades. In this case any change to the blade shape or size would need to be applied to ALL 'instances' which is exactly what would happen with the 'Pattern Face' function and without the overhead of having to create 5 additional fully-featured copies of the original set of features.
Also note that 'Pattern Face' has been part of NX for some time, first as a very basic function then it was moved to the Synchronous Modeling suite of tools and finally, in NX 9.0, being given the same basic Dialog look and feel as Pattern Feature which was introduced in NX 8.0. And while were at it, in NX 9.0 we also replaced Instance Geometry and Component Arrays with their own 'Pattern' functions again using the now common 'Pattern' dialog design and behavior. This way, once a user becomes familiar with how one 'Pattern' function works, he will be able to quickly learn to use any of the other 'Pattern' functions since they will share the same basic dialog design, and where appropriate, a common set of options and features.
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.
Also note that 'Pattern Face' has been part of NX for some time, first as a very basic function then it was moved to the Synchronous Modeling suite of tools and finally, in NX 9.0, being given the same basic Dialog look and feel as Pattern Feature which was introduced in NX 8.0. And while were at it, in NX 9.0 we also replaced Instance Geometry and Component Arrays with their own 'Pattern' functions again using the now common 'Pattern' dialog design and behavior. This way, once a user becomes familiar with how one 'Pattern' function works, he will be able to quickly learn to use any of the other 'Pattern' functions since they will share the same basic dialog design, and where appropriate, a common set of options and features.
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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