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Intersect a body with a sheet
- Thread starter NXJockey
- Start date
If by doing so you intend to create a curve then as long as they physically intersect then you can create an intersection curve. If you wish to trim one using the other then they must not only intersect but be manifold.
There are slight variations on those themes but I suspect you'll need to clarify just a little as to what sort of result you desire.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
There are slight variations on those themes but I suspect you'll need to clarify just a little as to what sort of result you desire.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
JohnRBaker
Mechanical
And then doing what with the Solid body and Sheet body?
If by "intersecting" you mean to join them together to make a single body, probably NO, not in that sense. Can one be used as a tool to modify the other, then perhaps YES, depending on what it is that you expect the operation to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
If by "intersecting" you mean to join them together to make a single body, probably NO, not in that sense. Can one be used as a tool to modify the other, then perhaps YES, depending on what it is that you expect the operation to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #4
A little more info......
I wish to create a partial planar section thru a solid body,
I cant use the section command and select specific faces of the solid, because as the design evolves, the faces may not be in the area i am interrogating with the section.
I dont want to section the whole solid, as there are 1000's of surfaces in it, which will take along time to evaluate which surfaces to intersect, then intersect 100's of faces which i am not interested in, which will increase part file size and degrade performance.
The only way i have thus far of doing this is to wave link te solid into a parent part, then intersect this linked body with a surface, but using the feature option in the selection intent to select the linked solid.
I have no method to do this all in the same part.
Come on chaps..... I feel an ER comming on.......
NXJ
I wish to create a partial planar section thru a solid body,
I cant use the section command and select specific faces of the solid, because as the design evolves, the faces may not be in the area i am interrogating with the section.
I dont want to section the whole solid, as there are 1000's of surfaces in it, which will take along time to evaluate which surfaces to intersect, then intersect 100's of faces which i am not interested in, which will increase part file size and degrade performance.
The only way i have thus far of doing this is to wave link te solid into a parent part, then intersect this linked body with a surface, but using the feature option in the selection intent to select the linked solid.
I have no method to do this all in the same part.
Come on chaps..... I feel an ER comming on.......
NXJ
JohnRBaker
Mechanical
And what's stopping you from selecting the solid body as a 'feature' in the original part file?
I see no advantage of sectioning an associative copy of a solid in terms of getting a different result. Granted, by using the WAVE-linked copy, you save adding a feature to your original model and it does provide more control over when you wish the section to update, but the resulting model will be identical if you do not make any changes to the WAVE-linked body before you create your section.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
I see no advantage of sectioning an associative copy of a solid in terms of getting a different result. Granted, by using the WAVE-linked copy, you save adding a feature to your original model and it does provide more control over when you wish the section to update, but the resulting model will be identical if you do not make any changes to the WAVE-linked body before you create your section.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
I'm not sure if I understand the question but here is my 2 cents. You can intersect a sheet with a solid body if you choose the sheet as the target and the solid body as the the tool. If you wish to keep the solid body intact, select the "Keep Tool" option in the dialogue box
- Thread starter
- #7
Cheers mmauldin,
I see what you have done, & thanks,
You result generates a trimmed surface, I only really needed curves, the same as the output from the section or intersection commands with the curves from bodies toolbar.
I check out what this method does to performance & part file size on some really large models.
I found a old grip program which itersects a body with a surface to give curves, but the result is explicit
John, I might raise this as a ER anyway, as the command would be ever so easy to create as all the parts are already there in NX. They just need bringing together.
Cheers,
NXJ
I see what you have done, & thanks,
You result generates a trimmed surface, I only really needed curves, the same as the output from the section or intersection commands with the curves from bodies toolbar.
I check out what this method does to performance & part file size on some really large models.
I found a old grip program which itersects a body with a surface to give curves, but the result is explicit
John, I might raise this as a ER anyway, as the command would be ever so easy to create as all the parts are already there in NX. They just need bringing together.
Cheers,
NXJ
JohnRBaker
Mechanical
Trust me, unless you can provide a much clearer idea of that what exactly it is that you are attempting to do and reasons why existing functions are not up to the task, any ER submitted will not get a very high priority. Can you at least provide us with a picture of what it is that you need?
You keep saying 'sheet body' yet at the same time you talk about a 'planar section'. So why aren't you using a Datum Plane instead of creating a Sheet Body to use as your sectioning tool?
Also (and this goes for EVERYONE), when you are talking about some specific task or operation, PLEASE tell us what version of NX that it is that you're running. Things change from one release to next and it gets difficult to make a recommendation if we don't know where you are in terms of the change history of the software.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
You keep saying 'sheet body' yet at the same time you talk about a 'planar section'. So why aren't you using a Datum Plane instead of creating a Sheet Body to use as your sectioning tool?
Also (and this goes for EVERYONE), when you are talking about some specific task or operation, PLEASE tell us what version of NX that it is that you're running. Things change from one release to next and it gets difficult to make a recommendation if we don't know where you are in terms of the change history of the software.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
If what you want to do is unite the sheet with the body (as previously stated) the answer is no.
But I may have a tip:
If you add a thickness to the sheet (use "thicken") you will have a solid body and you can then unite it. You only need to thicken it a tiny bit (a ten-thousandth of a unit, or maybe even less) to make it a solid.
But I may have a tip:
If you add a thickness to the sheet (use "thicken") you will have a solid body and you can then unite it. You only need to thicken it a tiny bit (a ten-thousandth of a unit, or maybe even less) to make it a solid.
- Thread starter
- #11
All,
In answer to your questions.
I am currently using NX4 (32 os), but have also tried this on NX6 with the same problem. I am sure that I have done this in NX2, but my memory is not what is was
and I could be thinking of another CAD tool.
I am working on an ‘extremely’ complex casting with lots of free form surfaces in it. The model as a whole, has been optimised as much as possible to remove excessive parameterisation.
I am trying to define the best positions through various ribs etc for passageways. These passageways are not straight, nor will they have constant wall thickness in relation to the cast faces, due to various thermal & structural restrictions.
What I typically do is define the passage way cross-sections at key locations, then link all of the cross sections together. (It’s not that hard really!!) just laborious. It’s a bit like doing a core on a turbine blade in a gas turbine engine. But the external casting I am currently working with is as complex as a turbine blade, but there’s a lot more of it with multi directional passage ways.
I typically create the sections through the solid body using the section command, under ‘insert curve from bodies’. This works fine on small non complex bodies as the results return quickly and the effect on part file size is manageable.
I then use these curves to position curves within a sketch, which has been defined on the datum which was used to create the section in the first instance.
The problem I now have is the complexity of the body, if I section using a plane (infinite in size) it sections through the whole solid body, most of which is not in the region I am working, which takes a long time and is really inflating the part file size.
I could extract a copy of the body, which then makes a feature, then use this feature as the input (using the appropriate selection intent modifier) in the ‘insert > curve from bodies > intersect’ to intersect the feature with my bounded plane surface. This gives the result as curves. But…………extracting the body increases the part file size. I could extract individual faces & sew them together, but again it increases the part file size & gets messy.
So it seemed logical to me, to create a simple planar surface ‘bounded plane’ in the region I need the section. The theory being that NX will only section to the extents of my bounded plane.
The point I am trying to make is, if the selection intent options in the ‘insert > curve from bodies > intersect’ command had a option ‘body’ this would all work, (again I’m sure I have done this operation before)
Mmauldin’s suggestion is pretty much there, but like I said, I want to do some tests to check the performance and effect on part file size. After all, it takes more data to store a surface that it does simple curves. Therefore it would be fair to assume that it would take longer to create the section ‘surface’ than the section ‘curves’. This could also affect regeneration times. But I need to test this (I’ll let you know what I find out).
I’ll knock up a simplified example of what I am trying to achieve. As I cant show you the real thing.
This thread seems to got people’s interest going, I guess it sounds easy in theory.
Cheers,
NXJ
In answer to your questions.
I am currently using NX4 (32 os), but have also tried this on NX6 with the same problem. I am sure that I have done this in NX2, but my memory is not what is was
and I could be thinking of another CAD tool.I am working on an ‘extremely’ complex casting with lots of free form surfaces in it. The model as a whole, has been optimised as much as possible to remove excessive parameterisation.
I am trying to define the best positions through various ribs etc for passageways. These passageways are not straight, nor will they have constant wall thickness in relation to the cast faces, due to various thermal & structural restrictions.
What I typically do is define the passage way cross-sections at key locations, then link all of the cross sections together. (It’s not that hard really!!) just laborious. It’s a bit like doing a core on a turbine blade in a gas turbine engine. But the external casting I am currently working with is as complex as a turbine blade, but there’s a lot more of it with multi directional passage ways.
I typically create the sections through the solid body using the section command, under ‘insert curve from bodies’. This works fine on small non complex bodies as the results return quickly and the effect on part file size is manageable.
I then use these curves to position curves within a sketch, which has been defined on the datum which was used to create the section in the first instance.
The problem I now have is the complexity of the body, if I section using a plane (infinite in size) it sections through the whole solid body, most of which is not in the region I am working, which takes a long time and is really inflating the part file size.
I could extract a copy of the body, which then makes a feature, then use this feature as the input (using the appropriate selection intent modifier) in the ‘insert > curve from bodies > intersect’ to intersect the feature with my bounded plane surface. This gives the result as curves. But…………extracting the body increases the part file size. I could extract individual faces & sew them together, but again it increases the part file size & gets messy.
So it seemed logical to me, to create a simple planar surface ‘bounded plane’ in the region I need the section. The theory being that NX will only section to the extents of my bounded plane.
The point I am trying to make is, if the selection intent options in the ‘insert > curve from bodies > intersect’ command had a option ‘body’ this would all work, (again I’m sure I have done this operation before)
Mmauldin’s suggestion is pretty much there, but like I said, I want to do some tests to check the performance and effect on part file size. After all, it takes more data to store a surface that it does simple curves. Therefore it would be fair to assume that it would take longer to create the section ‘surface’ than the section ‘curves’. This could also affect regeneration times. But I need to test this (I’ll let you know what I find out).
I’ll knock up a simplified example of what I am trying to achieve. As I cant show you the real thing.
This thread seems to got people’s interest going, I guess it sounds easy in theory.
Cheers,
NXJ
Yours seems to me top be more a problem of compartmentalising the design task than anything. It may suffice to create an extrusion encapsulating the affected area that you wish to work in and then use it to temporarily create an intersection solid so that you can just work in the area that affects you until you get it right. That solid could easily be sectioned quite effectively and worked on in a way that may be easier for you.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
JohnRBaker
Mechanical
I think I'm finally figuring out what you're trying to do, but let me see if I've got this right.
You have a large complex solid (a casting) and you would like to extract a planar set of curves based on the intersection of a plane (or planar surface) and ONLY SOME OF THE FACES of the body, but you don't want to have to select each face one at a time since there could be several hundred of them. Is that about it?
Now you can do that in NX 4.0 but you'll have to use...
Insert -> Curves from Bodies -> Intersect...
...and for the selection of the faces you can use the Selection Intent option 'Region Faces' where you select a single 'seed face' (which is one of the set of faces you wish to select) and then boundary faces to define the 'region' which bounds the set of faces you wish to include.
I created a video of the session, but I'm having problems uploading it, so if you have access to the GTAC site I can up load to our FTP 'scratch' area and you can download it from there. Just let me know and I'll move the file and let you know the name of it.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
You have a large complex solid (a casting) and you would like to extract a planar set of curves based on the intersection of a plane (or planar surface) and ONLY SOME OF THE FACES of the body, but you don't want to have to select each face one at a time since there could be several hundred of them. Is that about it?
Now you can do that in NX 4.0 but you'll have to use...
Insert -> Curves from Bodies -> Intersect...
...and for the selection of the faces you can use the Selection Intent option 'Region Faces' where you select a single 'seed face' (which is one of the set of faces you wish to select) and then boundary faces to define the 'region' which bounds the set of faces you wish to include.
I created a video of the session, but I'm having problems uploading it, so if you have access to the GTAC site I can up load to our FTP 'scratch' area and you can download it from there. Just let me know and I'll move the file and let you know the name of it.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
As a matter of fact if you created the extrusion that I mentioned as a way of defining a boundary that you wanted to work to then you could select a face to use in creating the intersected curves. Either that or creating a sketch to define a bounded plane, might help with John's suggested method.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
- Thread starter
- #15
Yes John,
Now you have got the idea.
The method you describe does work, and gives the desired curves,
The only problem is that it is could be laborious to select the boundaries for the seed. Lots of selections may be necessary. Using my dream command (can I have it please) I would only need two selections 'Solid - Bounded plane'.
One of the things which I promote is 'robust modelling' the theory goes that the model should be as robust as possible so support as many ‘unplanned’ topological changes as possible which in turn support concurrent engineering. Any time spend editing a model to 're-attache' bits and bobs which don’t regenerate properly is wasted time, hence wasted money.
- Thread starter
- #16
JohnRBaker
Mechanical
Yes, you have to be careful in your selection of a Seed face so that it's one that is not likely to be deleted or replaced as a result of editing or deleting some previous feature in the model's history, but that does not make the 'Region Faces' a particularly unattractive or poor mechanism. Note that this use of Seed/Boundary faces is a very old concept and predates it's current use as a general Selection Intent method by many years (back to at least UG V16.0) as it was always the primary selection mechanism for Simplify Body (which has since been replaced by Delete Face) and has always proved to be both reliable and usable. Granted, on very complex models it could, as you pointed out, be a bit tedious when selecting the Boundary faces, but remember, this is a very general purpose selection mechanism and is useful with many more functions than just Intersection, so once mastered it can become quite useful simply because it does provide a very general mechanism which can account for significant changes to the original model and still be able to properly and reliably maintain your 'design intent'.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
JohnRBaker
Mechanical
The problem is that 'Body Faces' includes ALL faces of the model not just those in the area of interest. The 'Region Faces' selection intent option is really the recommended approach for the problem as originally stated.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John,
I realised but wondered if it would really slow things down overall as compared with the need that was mentioned to ensure that the region seed and/or boundaries remained valid.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
I realised but wondered if it would really slow things down overall as compared with the need that was mentioned to ensure that the region seed and/or boundaries remained valid.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
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