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Thread: Fusion360 Question: Moving a Sketch Element

  1. #1
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    Default Fusion360 Question: Moving a Sketch Element

    Here I am on my first attempt to design a part with Fusion360. So far I have three outlines in the X-Z plane: one that I created from scratch and two more that were made with the offset command so they are all on the same plane. The largest is supposed to be the bottom, the middle size is the outline of the top, and the smallest is to cut a hole about 3/4 of the way down from the top. I planned to use the Loft command to connect the bottom and top with sloping sides. Then add the hole. It all seemed so easy.

    So, I have the three outlines and I am trying to use the Move/Copy command to bring two of them up 1/2" so they are at the level of the top. But it does not work. I type in 0.5" for the Y axis but nothing moves. I have tried it about a dozen times using different variations, but nothing works. However, the UnDo button seems to think that the Move/Copy did happen because it offers me the option of UnDoing it. What am I doing wrong? Am I in the wrong workspace? Or what?

    Any suggestions?
    Paul A.

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    You can't win and there is a penalty for trying!

  2. #2
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    Hello Paul,

    Autodesk Inventor user here, but they are similar. Maybe the first outline (from which you offset the others I presume) was automatically constrained to the origin point? You may have to delete the constraint before you can move it? Just a suggestion.

    Ian.

  3. #3
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    If it was me I would create my bottom on the XZ plane and then insert an offset plane at the height of the top and sketch the top on the offset plane. Then end the sketch and loft between the two. The hole I would make wherever you wanted it.
    How to become a millionaire: Start out with 10 million and take up machining as a hobby!

  4. #4
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    What Black Forest said; you'll want to create the top sketch on a user defined plane. Right now, the sketches are constrained to the planes on which they were designed.

    For the hole, do the sketch after the lofted solid is created, selecting the top surface to sketch on. You can then draw the circle, dimension its location, and do a negative .75 extrude.

    Like machining, there are always lots of ways to go about things and Fusion has a lot of options to choose from. I can't remember the last time I lofted a shape though, I find it easier to create solids like you would machine them, start with a lump and then whittle away for the features. Depending on the shape, of course, putting all the features into the initial sketch can make it harder to go back and change individual features.
    George

  5. #5
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    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.

  6. #6
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    Another way of saying the requirements for lofting is the geometry must be in different sketches which are on different planes.

    Starting from your original sketch with the offsets, create an offset plane the correct height above the original sketch plane for the first offset. Create a sketch on the plane. Project the first offset to that sketch. Repeat process for the second offset.

  7. #7
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    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.
    Last edited by J Tiers; 11-13-2017 at 02:45 PM.
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  8. #8
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    A loft is useful for joining two dis-similar shapes. Or for creating more "freeform" connections rather than just simple flat faces. Since you stated that the two sketches are created by the offset command then I assume they are the same, just "scaled". And being a newby, I'm going to assume your not trying to create a fancy swoopy shape with the loft?
    In that case, just a simple extrude with a negative draft (fusion calls it a taper angle) is all you need to make the initial shape from one single sketch.
    You could also extrude the base shape straight up, and add the draft as a second operation too. this would be useful if you would want to draft the walls at different angles
    And as was said before, the hole from the top is a separate sketch and extrusion (using cut rather than add) built on top of that solid once its created.

  9. #9
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    Yes, in MOST cases, it will be better to do several sketches and extrudes etc, rather than trying to cram too much into one sketch, as commented by the other poster just previous concerning the hole.

    That makes it easier to edit, easier to understand, easier to try out things. It is MUCH easier if you are not sure about some feature, because usually, you can leave the sketch, and delete the feature just by deleting or suppressing the extrude. Then if you want to put it back, you need not re-draw it, just un-suppress it, or open the sketch and re-extrude it.

    I did not mention adding "draft" to the extrusion, since in the programs I use, that is do-able separately, and does not have to be done at the time of the extrude (although I believe you CAN do it then, I just never do).
    Last edited by J Tiers; 11-13-2017 at 06:11 PM.
    1601

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    Hashim Khan

  10. #10
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    First, thanks to all.

    I have read the replies once and feel that I need to go through them about five or ten more times, perhaps with some trial work in the program between readings. I'm stubborn and will probably be up to 2 or 3 AM with this.

    This is where I am after one additional try tonight. I could not see any way to specify a new plane to sketch on except to extrude from the original plane and them select the top surface of that extrusion. Is this the only way to get a new sketch plane? I need one that is 0.5" above the first one (X-Z in this case).

    Anyway, I did extrude using the two inner curves and got this:



    When I did that extrude, the outer curve which was to be the outline of my base disappeared. So then I drew a new base outline sketch on the original X-Z plane. But I can't seem to use the Loft command with that outline sketch and the outline of the extruded part in the photo. I am assuming that you must have two sketch outlines to use Loft, not a sketch and the edge of a solid.

    My problem, in my mind anyway, is that this part is based on the hole. My TV remote is supposed to fit in it. That is why I started with the inner curve and worked my way out. I am or at least want to work from the hole out, not the outside in. You can make out the three outlines in the photo: the first and inner one to fit the TV remote. It will be used to make a blind hole down, into the part. The second, middle outline which forms the top edge. And the third and outer outline which forms the bottom edge. I want a sloping surface between the top and bottom edges.

    It is beginning to sound like I need to draw that inner curve twice, once in the original X-Z plane, then extrude something to a plane that is 0.5" above it and draw it again in that plane. Then perhaps I can use the Offset command to generate the second and third curve from both of these. Delete the unwanted outlines on each plane and then use the Loft command. Would that work? Am I fighting the logic of the program?
    Paul A.

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

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