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Thread: Fusion360 Question: Moving a Sketch Element

  1. #21
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    Why would you use a taper, when loft is quite a bit simpler and can be done with only one sketch
    https://knowledge.autodesk.com/commu...a-a171f8b61081

  2. #22
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    Gary,

    I saw another video on using Loft and they did a great job of showing how those sketching planes can be moved around. I am picking this up one point at a time. And it seems that there are so many videos on Fusion360 that you can find multiple ones on just about any command you want. The only problem is knowing what words to include in the search.

    I have been using CAD for about 20 years or more but now I feel like a gross beginner again. On the good side, Fusion seems like a great program and you guys have been a great help. I suspect I got better and faster help here than I could have gotten from a Fusion forum. Thank you to all of you.



    Quote Originally Posted by garyhlucas View Post
    If you are an experienced 2d cad user you will struggle a bit to use parametric 3d modelers as most of what you know is mostly useless. Sketches are just that, sketching with no dimensions, then you apply constraints to the sketch in the form of dimensions and relations to origins etc. All sketches are done on planes, and only three planes exist initially, the X, Y, and Z. Sketches then get extruded or revolved to produce a solid. At that point every face can be used as a plane for a sketch. You can also create new planes using existing planes or surfaces as references to locate the new plane in 3d space. Then you continue sketching.

    Back to the original question. A sketch can only be moved in 2d on the plane or surface it was drawn on. To move it in the third dimension you must move the surface or plane it was drawn on, or create a new plane and move it there.

    Hope this helps.
    Paul A.

    Make it fit.
    You can't win and there is a penalty for trying!

  3. #23
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    There are "best practices" for CAD.

    And, there is the fact that any method that gets you to your desired endpoint is perfectly fair. Yes it may be better to use certain means as opposed to others.

    In this case, since you presumably had desired dimensions to hit at the top and bottom, you knew how high you wanted it, etc, you did what "I" would suppose to be probably the simplest overall method to get where you were going. It used the info you had, and directly got to the result you wanted.

    I'm not going to say that the alternate method is "wrong". It is an alternate way that probably will get to the same result. But to me it seems more confusing than a straightforward loft to get the outside shape. To the other poster, the way you (and I) would approach it may seem clumsy and confusing. And that is fine, let him do it his way, and you do things the way that you find more convenient, whether that is a loft or a drafted extrusion.

    If, for instance, you had NOT had the dimensions, but instead were given only bottom (or top) dimensions, and the angles, then the extrusion method might have directly used what info you had, and would be much simpler.

    The data you have drives the method, at least in terms of the most direct method (which may not be the best) and is why there are different ways to do many tasks in CAD. No one method fits all uses. It is a matter of understanding what you want, vs what you know, and picking a construction method based on that.

    I would not suggest putting a lot of faith in a statement that there is only one way to do a job, or even only one BEST way. The best way is the way that works, that you understand, that allows the easiest changes to those things you may want to change, and that has no big drawbacks
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  4. #24
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    J,

    As I said, I am re-reading everything here. I am sure there is a lot in your post but right now my mind is on what seems like a way of moving things around later in the process. I think you are saying that by adding a dimension, that dimension becomes a way of MOVING a feature at a later date. So, if I put a cube on top of a cylinder and add dimensions to show how far it is from the center or edge of that cylinder, then I can move that cube around by changing those dimensions at a later time. Is that what you are saying? That sounds like a powerful tool.

    I know there is more here and I will be reading it again, perhaps at a later date. I am going to save a link to this thread.



    Quote Originally Posted by J Tiers View Post
    You can , in 3D "parametric" cad, usually create a shape two ways.

    **** One: Extrusion

    You create a closed sketch. or two or more sketches defining a cross section, and then extrude it to some depth. The cross section remains the same for the whole depth of extrusion. So, a pipe would be two concentric circles, extruded to the needed depth.

    You can also cut with an extrusion, so a circle can cut a round hole to some depth, to a feature, or clear through a part, for instance. Any sketch that is closed can extrude a part, or do an extrude cut.

    **** Two: Lofting. This does shapes that change cross section.

    You create two or more sketches, each independent, on different planes and then tell the program to use those in a specific order to "loft", or create the part. The program shapes the part such that the cross sections define the surface at those planes, and the surface is "faired in" between them to create a smooth surface.

    The sketches are all usually separate, and you list them in the loft command. Most programs do not do multiple things in one sketch, a sketch is on one plane. Any other plane has to be a different sketch.

    You may also be able to add "guide curves" to help define the surface between the cross sections, the surface will follow both the sections and the guide curves. The curves obviously must intersect the section outlines.

    Again, you can usually do a "loft cut", removing he shape instead of adding it.

    But you always start with a sketch, which is done on a plane. If you use a basic plane, the plane is fixed. In some programs if you define another plane, you can move it and the shape will move to accommodate the new position when re-created.

    *****

    That is the effective meaning of "parametric", you can go back and edit the "parameters" and the part will change accordingly.

    Parameters are generally dimensions and constraints applied to the lines of a sketch, for single parts. Dimensions are lengths, diameters, angles etc. Constraints are making things concentric, parallel, tangent, touching, co-linear, etc with one or more other items (lines etc in sketches, but surfaces and centers, etc in assemblies).

    So if you decide the extrusion needs to be an inch longer, you can change that dimension, and the part is an inch longer.

    One key point is how that interacts with other parts in an assembly. Surfaces have names, usually a number like "surface 12" If you were to CUT the extrusion an inch shorter, or add a piece on, then the name of the surface at the end would change. If you had, in an assembly, that original surface contacting something, and then you cut off the end of the extrusion, the name will be gone, and the assembly will have a bad constraint, the things that you set to be in contact will not both exist, so your assembly may come apart unexpectedly, and you should have an error show up.

    BUT, if you change the length, the name stays the same, and the constraints in assemblies are not affected aside from the dimension change itself.

    When you do a sketch, you can put a shape down nearly anywhere. Then you DEFINE it by adding dimensions vs the origin, or vs some already created portion of a part, and also dimensions defining the sketch itself. So you can just draw a rectangle that you want to have one corner at the origin. Anywhere. Then you dimension the corner as a zero distance to the origin, and dimension the opposite sides of the rectangle as their distances from each other. Finally you make one side parallel to an axis. That sets the location, orientation, and size of the rectangle.

    Usually you can just start the corner at the origin, and you will have an "implied dimension" holding it there. Or you could separately define, say, the lower side as zero from the x axis, and the left side as zero from the Y axis, which locates the rectangle also. If you then dimension the height and width, it is fully located and defined.

    Just remember...... it is all about changing the "parameters". It is usually BEST to draw the shape away from where you want it, and set its location with dimensions. That way you know you finished the job of defining it.

    If you do NOT fully define the sketch, you may get away with it, but later, if you change something, the sketch might get literally "bent out of shape", as the undefined dimensions are changed to accommodate the change you made. If everything is defined, you know what will happen when you make a change.
    Paul A.

    Make it fit.
    You can't win and there is a penalty for trying!

  5. #25
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    Default Another Question: Yellow Line

    Somewhere along the way to getting my final(?) model last night one of my original lines for the edge of the hole turned yellow. Does that color have any significance? Is there any guide to what colors mean in Fusion?
    Paul A.

    Make it fit.
    You can't win and there is a penalty for trying!

  6. #26
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    Paul you really should join the Fusion forum. You will get answers from people that actually use the software you are trying to learn. And get it quick.
    How to become a millionaire: Start out with 10 million and take up machining as a hobby!

  7. #27
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    J,

    First, I am and know that I am a long, LONG way from "best practices" with Fusion. That will take time and practice. This is literally my very first attempt at a 3D part with it and I am very happy that I got at least one result so fast. That is thanks to all here who have provided the so much needed help. I am very grateful for that. This board is a great place with a great bunch of people.

    The main problem I seemed to have was how to go from the inside out, instead of from the outside in as most examples of 3D design seem to use. I wanted to start with the hole, which I could provide dimensions for, and work outward from there. So my outlines on all three construction planes were based on that initial hole size and shape. And I wound up drawing that sketch three times. I still think that there must be a way to copy a sketch from one plane to another. Ian is apparently talking about it above. I will be looking for it in my next efforts.




    Quote Originally Posted by J Tiers View Post
    There are "best practices" for CAD.

    And, there is the fact that any method that gets you to your desired endpoint is perfectly fair. Yes it may be better to use certain means as opposed to others.

    In this case, since you presumably had desired dimensions to hit at the top and bottom, you knew how high you wanted it, etc, you did what "I" would suppose to be probably the simplest overall method to get where you were going. It used the info you had, and directly got to the result you wanted.

    I'm not going to say that the alternate method is "wrong". It is an alternate way that probably will get to the same result. But to me it seems more confusing than a straightforward loft to get the outside shape. To the other poster, the way you (and I) would approach it may seem clumsy and confusing. And that is fine, let him do it his way, and you do things the way that you find more convenient, whether that is a loft or a drafted extrusion.

    If, for instance, you had NOT had the dimensions, but instead were given only bottom (or top) dimensions, and the angles, then the extrusion method might have directly used what info you had, and would be much simpler.

    The data you have drives the method, at least in terms of the most direct method (which may not be the best) and is why there are different ways to do many tasks in CAD. No one method fits all uses. It is a matter of understanding what you want, vs what you know, and picking a construction method based on that.

    I would not suggest putting a lot of faith in a statement that there is only one way to do a job, or even only one BEST way. The best way is the way that works, that you understand, that allows the easiest changes to those things you may want to change, and that has no big drawbacks
    Paul A.

    Make it fit.
    You can't win and there is a penalty for trying!

  8. #28
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    Quote Originally Posted by Paul Alciatore View Post
    J,
    I still think that there must be a way to copy a sketch from one plane to another. Ian is apparently talking about it above. I will be looking for it in my next efforts.
    There is more than one way to do this.
    1. Create a sketch on the new plane. Copy the geometry from the first sketch to the second.
    2. The preferred way is to use the Project command as it can be parametric, that is when the first sketch changes, the projected geometry will change.

  9. #29
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    Paul, think of 3D CAD as if you were machining the part. You start with a chunk of metal or plastic and whittle away at it. It helps to get the concept in your mind I find.
    How to become a millionaire: Start out with 10 million and take up machining as a hobby!

  10. #30
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    You actually CAN in many cases "whittle away" to get a part. Literally.

    I find it much easier to do it as a build-up, possibly in combination with some "whittling". But in many cases you could literally create a block, and then cut away whatever is not on your part.

    Quote Originally Posted by Paul Alciatore View Post
    J,

    First, I am and know that I am a long, LONG way from "best practices" with Fusion. That will take time and practice. This is literally my very first attempt at a 3D part with it and I am very happy that I got at least one result so fast. That is thanks to all here who have provided the so much needed help. I am very grateful for that. This board is a great place with a great bunch of people.

    The main problem I seemed to have was how to go from the inside out, instead of from the outside in as most examples of 3D design seem to use. I wanted to start with the hole, which I could provide dimensions for, and work outward from there. So my outlines on all three construction planes were based on that initial hole size and shape. And I wound up drawing that sketch three times. I still think that there must be a way to copy a sketch from one plane to another. Ian is apparently talking about it above. I will be looking for it in my next efforts.
    There often IS such a way. I do not specifically know Fusion, so I donlt know their way.

    There is also a way to develop a sketch from existing geometry in most. In Alibre it is called "project to sketch". You select edges on the model which then will be transferred to the current sketch plane as sketch lines. You generally have the choice of tying that to the shape, so that it is updated if the shape changes, or having it just transfer, with no updating.

    One way to do the transfer which is clumsy but should work, is to use a "throwaway extrusion".... extrude the sketch, then project from that extrusion to the new plane, finally delete teh extrusion. There is probably a simpler way, and you may be able to do it directly if Fusion allows multiple sketches to be open at once.

    As for best practices, they are often a royal pain in the neck, and can be ignored in many cases to "get out the production". There are technical reasons for them, but those are not always applicable. Sometimes you really DO need to use them, though.
    Last edited by J Tiers; 11-14-2017 at 04:09 PM.
    1601

    Keep eye on ball.
    Hashim Khan

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