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Point
- Thread starter vitulin
- Start date
- Thread starter
- #2
I gave this a go NX 5.0.3.2 what I found is that you can make a point in the sketcher by intersecting a curve with a datum plane, but it does not appear to behave in the same associative manner as does the same point created outside the sketcher. In either case the point is defined as a simple intersection pint by picking the datum plane first and a another object second. For the second object you would pick the curve but you could equally use an edge if you wish to.
I'm not sure why the sketched point isn't associative even if you model the curve inside the same sketch. However the fact that it still works outside the sketcher means that you can probably do whatever it is that you need because the sketcher will interact with that point. As far as I can tell there's nothing that you can't do because of the way this works. The only thing it may affect is the ease of linking your sketch to another model in that you'll have to link the points separately. Linked sketches are something I'd use sparingly at the best of times so I'm not bent out of shape over it.
Best Regards
Hudson
I'm not sure why the sketched point isn't associative even if you model the curve inside the same sketch. However the fact that it still works outside the sketcher means that you can probably do whatever it is that you need because the sketcher will interact with that point. As far as I can tell there's nothing that you can't do because of the way this works. The only thing it may affect is the ease of linking your sketch to another model in that you'll have to link the points separately. Linked sketches are something I'd use sparingly at the best of times so I'm not bent out of shape over it.
Best Regards
Hudson
- Thread starter
- #4
Yes, I found out exactly the same...with one small difference...While in sketcher, I cant pick the datum...when out of the sketcher, I can...On the other hand, also i sketcher, there is an option of creating associative point... but I didnt try it because it didnt let me to pick the datums...
JohnRBaker
Mechanical
There's a special function for defining the intersection point of a curve and the sketch plane as shown in the attached image.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
Okay this one is starting to get a bit annoying really. As I said I can get useful results by alternate methods, so whatever you need yo do, you can do it. But why you can't do certain things makes no sense to me and I'm hearing all this testing it out and wondering why.
Yesterday after I posted to Vit I realized that there is an extra option for creating associative point in the sketcher that I hadn't really checked out thoroughly in this particular case. When I did I found probably what Vit did, but maybe I can explain it better. I have a datum plane outside of the and before it in timestamp. The datum plane is normal to the plane of the sketch that I now create. Then I go into the sketcher and create a new curve using the sketcher. Now I can create a non-associative point between that new sketched curve and the datum plane, or I can use any curve or edge outside of the sketch. If I want to create an associative intersection point I can use curves or edges outside the sketch but if I attempt to select curves created within the same sketch it comes up with, "cannot select curves belonging to the active sketch". My question is why is this so?
My second attempt to do the same thing within the sketcher revolves around using the intersection point icon the John pointed out. So far as I can see while, based on the icon, it looks a bit like it might allow you to create an intersection point between a curve and any datum plane, it only creates an intersection between the plane of the sketch and curves that you can select. Hence when using the dialog you can only select curves because the sketch plane is already assumed. These points also have a funny habit of disappearing as soon as you finish sketching. I don't know what that means but they don't appear to be available to interact with anything else outside the sketch. In fact these intersection points appear to be of such very limited use that I guess there is some other specific intent which I'm missing. At any rate they do nothing like the test case that I was using so I'm back to the original answer.
The closest solution seemed to be to create an associative point outside the sketcher. As I said earlier this has few disadvantages that I could identify, even if for some it will be less appealing to have the extra feature in the model tree.
Your curiously
Hudson
Yesterday after I posted to Vit I realized that there is an extra option for creating associative point in the sketcher that I hadn't really checked out thoroughly in this particular case. When I did I found probably what Vit did, but maybe I can explain it better. I have a datum plane outside of the and before it in timestamp. The datum plane is normal to the plane of the sketch that I now create. Then I go into the sketcher and create a new curve using the sketcher. Now I can create a non-associative point between that new sketched curve and the datum plane, or I can use any curve or edge outside of the sketch. If I want to create an associative intersection point I can use curves or edges outside the sketch but if I attempt to select curves created within the same sketch it comes up with, "cannot select curves belonging to the active sketch". My question is why is this so?
My second attempt to do the same thing within the sketcher revolves around using the intersection point icon the John pointed out. So far as I can see while, based on the icon, it looks a bit like it might allow you to create an intersection point between a curve and any datum plane, it only creates an intersection between the plane of the sketch and curves that you can select. Hence when using the dialog you can only select curves because the sketch plane is already assumed. These points also have a funny habit of disappearing as soon as you finish sketching. I don't know what that means but they don't appear to be available to interact with anything else outside the sketch. In fact these intersection points appear to be of such very limited use that I guess there is some other specific intent which I'm missing. At any rate they do nothing like the test case that I was using so I'm back to the original answer.
The closest solution seemed to be to create an associative point outside the sketcher. As I said earlier this has few disadvantages that I could identify, even if for some it will be less appealing to have the extra feature in the model tree.
Your curiously
Hudson
JohnRBaker
Mechanical
There is a general architectural limitation that does NOT allow a 'feature' to be created inside of another 'feature'. What this means is that if we need to create anything that is associative to something outside the sketcher that it must be done with a sketch specific function such as the associated point function I've already pointed out. This is a hard and fast limitation and we're always working on more sketch specific tools with the idea that these will help to reduce the need to try to make non-sketch functions work inside the sketcher.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John,
I think that as long as the sketcher interacts with other features then that is okay, because it means you can do pretty much everything I imagine you might need to. At least it make sense and there's a reason for it, so you need to maintain one feature for an datum plane, one for an associative point, and then you can easily dimension or constrain relative to either or both.
I have been having a play with it and created some perfectly wonderful examples with no trouble at all. I was really happy with it and impressed by how easily it worked, so it isn't that I mean or meant to complain, I just don't understand a couple of things.
As I said earlier if I'm right in how I explained my experience of the intersection point with the sketch plane function, inside the sketcher, then I wonder what prompted it to be created in the first place. Obviously it is meant to be used for something, but it behaves rather strangely with the points disappearing when you leave the sketcher. So given that we accept the logic that certain associative points, arguably in the majority of cases, will need to be created outside the sketcher for reasons that seem logical, why then do we have this extra function unless it provides an extra capacity that could only be achieved in this way and inside the sketcher? Or in other words why not just make those points outside the sketcher too since it seems consistent with the rest of things?
The other more general thing is to clarify my/our understanding of what you mean when you say one feature should not be allowed to be created inside another feature. Where that line is drawn seems kind of fuzzy to me and while it is probably presumptuous of me to have expectations to understand anything at all there is that part of all of us that likes to know what to expect. So you can create geometry curves and points inside the sketcher and constrain them relative to one another and objects outside the sketcher, but to associate a point with any curve in the same sketch is somehow an impossible constraint. I might be being a bit dull today but it doesn't seem that different from some of the other possible constraints or I'm missing some point of difference that is vitally important to the software but completely non-apparent to the user. I'm wracking my brains to comprehend a circularity that I imagined may exist but I can't see one that isn't by analogy seeming equivalent to the other allowable sketch functions. So why then are we able to create associative points inside the sketcher only to objects outside the sketcher, and yet we can create a point in the sketcher and then constrain it to be point on curve with any two sketch curves or a sketch curve and the external plane and/or combinations of internal external objects, basically all of the above?
Vit,
Did you get that I think I answer the question. Just create a non-associative point then constrain it to be point on curve to both objects and darned if it isn't equivalent to an associative intersection point.
Best Regards
Hudson
P.S. Part of me hopes I'm really wrong about this one and that I ought to stand corrected, otherwise it works but it just doesn't make sense.
Best Regards
Hudson
I think that as long as the sketcher interacts with other features then that is okay, because it means you can do pretty much everything I imagine you might need to. At least it make sense and there's a reason for it, so you need to maintain one feature for an datum plane, one for an associative point, and then you can easily dimension or constrain relative to either or both.
I have been having a play with it and created some perfectly wonderful examples with no trouble at all. I was really happy with it and impressed by how easily it worked, so it isn't that I mean or meant to complain, I just don't understand a couple of things.
As I said earlier if I'm right in how I explained my experience of the intersection point with the sketch plane function, inside the sketcher, then I wonder what prompted it to be created in the first place. Obviously it is meant to be used for something, but it behaves rather strangely with the points disappearing when you leave the sketcher. So given that we accept the logic that certain associative points, arguably in the majority of cases, will need to be created outside the sketcher for reasons that seem logical, why then do we have this extra function unless it provides an extra capacity that could only be achieved in this way and inside the sketcher? Or in other words why not just make those points outside the sketcher too since it seems consistent with the rest of things?
The other more general thing is to clarify my/our understanding of what you mean when you say one feature should not be allowed to be created inside another feature. Where that line is drawn seems kind of fuzzy to me and while it is probably presumptuous of me to have expectations to understand anything at all there is that part of all of us that likes to know what to expect. So you can create geometry curves and points inside the sketcher and constrain them relative to one another and objects outside the sketcher, but to associate a point with any curve in the same sketch is somehow an impossible constraint. I might be being a bit dull today but it doesn't seem that different from some of the other possible constraints or I'm missing some point of difference that is vitally important to the software but completely non-apparent to the user. I'm wracking my brains to comprehend a circularity that I imagined may exist but I can't see one that isn't by analogy seeming equivalent to the other allowable sketch functions. So why then are we able to create associative points inside the sketcher only to objects outside the sketcher, and yet we can create a point in the sketcher and then constrain it to be point on curve with any two sketch curves or a sketch curve and the external plane and/or combinations of internal external objects, basically all of the above?
Vit,
Did you get that I think I answer the question. Just create a non-associative point then constrain it to be point on curve to both objects and darned if it isn't equivalent to an associative intersection point.
Best Regards
Hudson
P.S. Part of me hopes I'm really wrong about this one and that I ought to stand corrected, otherwise it works but it just doesn't make sense.
Best Regards
Hudson
JohnRBaker
Mechanical
OK, let's try and settle this issue of how 'points' should behave in the sketcher.
First, a point (excuse the pun) of clarity. The points created using that function I pointed out where you can find the intersection of some external curve and the plane of the sketch, was done strictly for internal purposes so that a user could constrain curves (via their endpoints to an existing point) to where the sketch intersected reference curves particularly when creating a sketch on (normal to) a curve or edge, such as needed when constructing a V-Sweep surface (introduced in NX 4).
But back to the issue of creating actual associative points in the sketch straight away. However, before we go any further let me inform all of you that we have taken what might appear to some to be a drastic action in that for NX 6 we've removed altogether the so called 'smart point' (associative) from the sketcher. In NX 6 you will only be able to create dumb points. The reason for this is that if you did create a smart point INSIDE the sketcher and then you tried to use that point in some manner to constrain some other object or you tried to then project that point onto the sketch plane, if it were no already on the plane, you would end getting either a warning about circular references or an error message about invalid ID's and so on. So that's why we removed that option altogether in NX 6. Now don't worry, if you've created a sketch with smart points in them and they have not cause any problems, those sketches will still open in NX 6 and their behavior will be consistent with what it was in NX 5, just that you will not get a chance to create new 'smart points' in the sketch.
Now that we have that out of the way, how is that we're expected to use points in the sketcher? Well remember when I mentioned that architecturally we can't have 'features' inside the sketcher. Well the issue is that the sketch has it's own 'parametric/associativity' environment and it does NOT use what we call 'feature methods', but rather 'constraints and relationships'. Now before we go any further note that a SKETCH is treated as a 'Feature' in to it has a place in the update tree and that it updates in time-stamp order and so on, but that what happens INSIDE the sketch is not known to the feature model, only what the final state is. To the rest of NX, a sketch is like a little 'black box'. You put something in, a change or edit, and something comes out, an altered profile/curves/points. What happened inside is a mystery, but as long as the modeler knows how to respond to the changed profile/curves/points the modeler doesn't care what actually happened inside the 'box'. BTW, that one reason why when you enter the Sketcher we 'suspend' the rest of NX and put the user into a 'task' where he can only perform sketch related operations, along with of course any appropriate 'special functions' such as viewing operations, hide/show, etc.
But getting back to what do we do with points. Well we treat them just link ANY other piece of geometry. After all, we don't really create 'smart' lines or arcs either, but rather object that we can constraint and define relationships between, and key word here is 'BETWEEN', since inside the sketcher, there are NO parent/child relationships to other sketch objects (with the possible exception of the new offset curve, but even then it's not 'time-stamp' sensitive). Inside the sketcher, all constraints and relationships are defined as a series of simultaneous equations which are solved as once to get a solution and since there is no need to solve every relationship since there are no parent/child issues, we can have under-constrained sketches or even ones with no constraints at all. So if points are just like a line or an arc, then we must use constraints to create the relationships that we desire and which will then update the way to wish them to.
So for example, let's take you example of the datum plane normal the plane of the sketch with which you wished to create an 'associative' point between that and one of the curves in my sketch. Now as long as the datum plane was created before the sketch in terms of the 'Time Stamp', you will be able to select the datum while editing the sketch. So what you do is either create an intersection point or just a point at a screen location since their not associative anyway who cares how the original point was actually created. Then go into assign Constraints and select the point and the curve of interest and create a 'Point on Curve' constraint and then repeat this with the point and the datum, again creating a 'Point on Curve' constraint (the datum, since it intersects the plane of the sketch, is treated as it it were merely a 'line'). Now that the point has been constrained, it will update if either the curve or the datum plane is modified.
Anyway, that's how it works and hopefully some insight into the why as well.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
First, a point (excuse the pun) of clarity. The points created using that function I pointed out where you can find the intersection of some external curve and the plane of the sketch, was done strictly for internal purposes so that a user could constrain curves (via their endpoints to an existing point) to where the sketch intersected reference curves particularly when creating a sketch on (normal to) a curve or edge, such as needed when constructing a V-Sweep surface (introduced in NX 4).
But back to the issue of creating actual associative points in the sketch straight away. However, before we go any further let me inform all of you that we have taken what might appear to some to be a drastic action in that for NX 6 we've removed altogether the so called 'smart point' (associative) from the sketcher. In NX 6 you will only be able to create dumb points. The reason for this is that if you did create a smart point INSIDE the sketcher and then you tried to use that point in some manner to constrain some other object or you tried to then project that point onto the sketch plane, if it were no already on the plane, you would end getting either a warning about circular references or an error message about invalid ID's and so on. So that's why we removed that option altogether in NX 6. Now don't worry, if you've created a sketch with smart points in them and they have not cause any problems, those sketches will still open in NX 6 and their behavior will be consistent with what it was in NX 5, just that you will not get a chance to create new 'smart points' in the sketch.
Now that we have that out of the way, how is that we're expected to use points in the sketcher? Well remember when I mentioned that architecturally we can't have 'features' inside the sketcher. Well the issue is that the sketch has it's own 'parametric/associativity' environment and it does NOT use what we call 'feature methods', but rather 'constraints and relationships'. Now before we go any further note that a SKETCH is treated as a 'Feature' in to it has a place in the update tree and that it updates in time-stamp order and so on, but that what happens INSIDE the sketch is not known to the feature model, only what the final state is. To the rest of NX, a sketch is like a little 'black box'. You put something in, a change or edit, and something comes out, an altered profile/curves/points. What happened inside is a mystery, but as long as the modeler knows how to respond to the changed profile/curves/points the modeler doesn't care what actually happened inside the 'box'. BTW, that one reason why when you enter the Sketcher we 'suspend' the rest of NX and put the user into a 'task' where he can only perform sketch related operations, along with of course any appropriate 'special functions' such as viewing operations, hide/show, etc.
But getting back to what do we do with points. Well we treat them just link ANY other piece of geometry. After all, we don't really create 'smart' lines or arcs either, but rather object that we can constraint and define relationships between, and key word here is 'BETWEEN', since inside the sketcher, there are NO parent/child relationships to other sketch objects (with the possible exception of the new offset curve, but even then it's not 'time-stamp' sensitive). Inside the sketcher, all constraints and relationships are defined as a series of simultaneous equations which are solved as once to get a solution and since there is no need to solve every relationship since there are no parent/child issues, we can have under-constrained sketches or even ones with no constraints at all. So if points are just like a line or an arc, then we must use constraints to create the relationships that we desire and which will then update the way to wish them to.
So for example, let's take you example of the datum plane normal the plane of the sketch with which you wished to create an 'associative' point between that and one of the curves in my sketch. Now as long as the datum plane was created before the sketch in terms of the 'Time Stamp', you will be able to select the datum while editing the sketch. So what you do is either create an intersection point or just a point at a screen location since their not associative anyway who cares how the original point was actually created. Then go into assign Constraints and select the point and the curve of interest and create a 'Point on Curve' constraint and then repeat this with the point and the datum, again creating a 'Point on Curve' constraint (the datum, since it intersects the plane of the sketch, is treated as it it were merely a 'line'). Now that the point has been constrained, it will update if either the curve or the datum plane is modified.
Anyway, that's how it works and hopefully some insight into the why as well.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John,
Thanks for the explanation. I guess that is the D-Cubed PGM thing that I have read about and was hitherto meaningless to me. I guessed that there was some risk of circular relationships being capable of being defined. To be honest I'm more concerned to understand how and where they come about in order to avoid cases where you're more or less likely to model yourself into a corner where you have to break the parameters in order to continue.
I also wondered if there wouldn't need to be a change to this just to make it at least appear more consistent. Once I discovered that you could constrain the point on a curve in two places to effectively achieve an associative intersection point I wondered whether it shouldn't be done that way all the time. Surely if the problems aren't likely unless the points are able to be created off the sketch plane, whereas in the majority of cases people would want to create these associative points only on the sketch plane, then there should be some way to support the valid case. That is to say it could be done either by actually automating the associative intersection point function within the sketch such that it simply constrains the point to be on the two curves provided they're on the sketch plane, and/or to change the name so that people understand what to expect, i.e. rather than intersection point call it constrain to two curves. By doing this either in the sketch point creation dialog, or as a constraint type you appear to still provide the capability, which you have anyway, but make it easier to use and accessible to users of the sketcher.
In the meantime I'm just as happy to accept the argument that there should be no way to create an associative intersection point within the sketcher, as it seems to be doubling up on functionality anyway. Which isn't to say that I think the the creation of a non-associative intersection point is a good idea since I think users would expect within the sketcher that it infer some kind of constraint according to how it was created. That is why I made some presumptuous suggestions above.
Best Regards
Hudson
Thanks for the explanation. I guess that is the D-Cubed PGM thing that I have read about and was hitherto meaningless to me. I guessed that there was some risk of circular relationships being capable of being defined. To be honest I'm more concerned to understand how and where they come about in order to avoid cases where you're more or less likely to model yourself into a corner where you have to break the parameters in order to continue.
I also wondered if there wouldn't need to be a change to this just to make it at least appear more consistent. Once I discovered that you could constrain the point on a curve in two places to effectively achieve an associative intersection point I wondered whether it shouldn't be done that way all the time. Surely if the problems aren't likely unless the points are able to be created off the sketch plane, whereas in the majority of cases people would want to create these associative points only on the sketch plane, then there should be some way to support the valid case. That is to say it could be done either by actually automating the associative intersection point function within the sketch such that it simply constrains the point to be on the two curves provided they're on the sketch plane, and/or to change the name so that people understand what to expect, i.e. rather than intersection point call it constrain to two curves. By doing this either in the sketch point creation dialog, or as a constraint type you appear to still provide the capability, which you have anyway, but make it easier to use and accessible to users of the sketcher.
In the meantime I'm just as happy to accept the argument that there should be no way to create an associative intersection point within the sketcher, as it seems to be doubling up on functionality anyway. Which isn't to say that I think the the creation of a non-associative intersection point is a good idea since I think users would expect within the sketcher that it infer some kind of constraint according to how it was created. That is why I made some presumptuous suggestions above.
Best Regards
Hudson
- Thread starter
- #12
Thanks for the answers. The problem with the outside of sketcher points is, that the tree is growing and growing. It would be perhaps fine, if there was similar option like in proe where you can create a group of points and it takes just one place in tree.
Regards
Vit
Regards
Vit
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