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Another loft that doesn't work!

Discussion in 'General Discussion' started by DaveD44, Aug 8, 2019.

  1. DaveD44

    DaveD44 Member

    I've spent hours trying to create a loft with various types of guide curves--2D and 3D splines included. Nothing works; no loft is created. I get the message: "ACISERROR_SKIN_GUIDE_NOT_INTERSECT: The guide curve does not intersect all profiles". If I leave out the guide curve I get a nice straight loft. See Loft 25 in the attached drawing. There must be a simple answer to this and I am missing it. Perhaps it has to do with the points I have defined, but there are seven in all and none appear to be duplicated in any one spot. As part of trying to get this to work I would like to un-constrain the guide curve(s) to the sketch points, but can't do that. I am trying to constrain the guide curve(s) to the sketches using the Coincident Constraint. Should I do it some other way?

    Attached Files:

  2. simonb65

    simonb65 Alibre Super User

    Zoom right in and look at your guide curve. It doesn't end on the points (which are on the corners of your target sketches) !
  3. simonb65

    simonb65 Alibre Super User

  4. DaveD44

    DaveD44 Member

    Well, but it does! Look at the measurement of distance of the top of the spline curve to the sketch at handle top. It's similar at the bottom. How close will Alibre allow me to put it. This it totally zoomed in.

    Of course, there are other problems evident here. Like just what is Reference Line<27>? I can't identify it directly on the drawing, but I suppose it is related to the sketch "Sketch xsect at handle top" to which I am attempting to attach the spline. It would be nice if I knew that this point was directly on the corner of this sketch, that is at the point the sketch lines end and connect together, but how to I tell?

    With all the waddling around that the display does when zooming in almost infinitely it is difficult to determine whether I really am putting these points on the sketch corner nodes as I am attempting to do when placing the points. They should be exactly there, but how can I really be sure that they are, with all the misalignment that happens when zooming way in. And this appears to be the problem.

    Are you also on Alibre 2019? I am running "Alibre Design™ Professional Version: 2019 64-bit [Build 20050]", which I suppose is the 2nd update to 2019 that I installed just a few days ago, but how can I tell? There is a disconnect between the update level (2019.0.2, or whatever) and what is displayed in the "About".

    And, again, just what is the proper way to connect the spline to the sketch corners? Is it Coincident Constraint? And how do I remove these constraints and, if necessary, the points that are associated with the sketch corner nodes? All this kind of activity is necessary if I am to debug my work effectively. And I won't even mention the cryptic error descriptions!

    Thanks anyway and sorry for the outburst.

    alibre point alighment.JPG
  5. HaroldL

    HaroldL Alibre Super User

    A couple of pointers...Place ALL Points in each of the Profile sketches. there is one in "Sketch xsect at handle top" that is not so I replaced it.
    When you sketch the Guide Curves make sure that when you place the start and end nodes that the Point highlights as in the image below. You may need to apply a Coincident constraint on it if you miss.

    I only used two guide curves for this image but making sure the guide curve end points were connected is key.

    Attached Files:

  6. simonb65

    simonb65 Alibre Super User

    It's displayed in the bottom right corner of the Home screen ...


    The .0.2. bit of the version is not important as the build number is 100% unique.

    Try panning around the intersection. It may look connected in one direction, but it isn't in others! The measurement tool rounds to 5 decimal places. Unfortunately the geometry engine works to much more accuracy than is displayed to the user ... and if it ain't equal, it ain't equal!

    Suggest you try the method @HaroldL suggests as the only way to get those exactly equal are by a coincident constraint.
  7. DaveD44

    DaveD44 Member

    After Simon's responses I decided to fiddle with it again and got it working. It was pretty apparent to me earlier that even though the sketch corners and the points defined there were right on the target, the problem was just as the error indicated and Simon verified that. You may note in the uploaded part that I had tried many things, none with success (the 2D and 3D sketches and splines above Loft<25>). So I went back to the loft with only a single guide curve, the spline for outside front (as in the uploaded part file) and worked with the handle top sketch. I will describe in detail the steps I took here because I still have some major concerns about why this doesn't work more easily and, as indicated in the thread title, this isn't the first thread discussing problems with lofts. I would like for something to come out of this discussion that may help in the future.

    From the uploaded part file, I turned on View References and un-suppressed Extrusion <18>, the underlying loft base.
    I then edited "Sketch xsect at handle top", part of the loft.
    I deleted the lock constraint on the left horizontal line of the sketch.
    I zoomed wayyyyy in on the lower corner and found that this corner and its associated point were visibly but an unmeasurable distance to the right of the geometry below it.
    I clicked on Coincident Constraint, selected the lower left corner of the geometry below, then the lower left corner of my sketch. Nothing.
    I then hovered over the left vertical line on the underlying geometry and it turned to a thin blue line. I then left clicked on it in select mode and, lo and behold, discovered that I could "Project to Sketch" that edge as a reference line. I did so. (I looked but could find no Alibre documentation that described the capability to project to sketch simply by clicking on a portion of background geometry.)
    I retried the constraint and after several tries it worked. However, the point associated with the sketch corner did not move.
    I deactivated sketch mode and had a successful loft!

    Back to the original sketches and guide curves. After having problems with an earlier loft (discussed elsewhere in this forum) I did, or thought I did, everything right with this one, including defining points on the two loft end sketch corners and constraining the ends of the guide curves to their respective points on the sketches. Yes, Simon, when it didn't work, I tried many times to again constrain them, but was unsuccessful. And yes, Harold, I had earlier deleted the point on the right for some reason (the one you restored) but hadn't bothered to replace it since I was working with the lower left exclusively. (The loft really needs only a single guide curve to look like it should.)

    So what was going on here? Is the guide curve actually constrained to the corner of the underlying geometry instead of the corner point of the handle sketch and moving the sketch over to that location made it complete? I had previously tried everything including advice in other threads and what both Simon and Harold suggested here, and nothing worked until I added a reference from the edge of the underlying geometry and moved the sketch to that location. I can't help but conclude that there is an underlying bug in Alibre that makes this difficult to do.

    Finally, Simon, I can also see the build number in the "About" display. The reason for wanting to see the build "0.2" or whatever number it happens to be is because I can't find a direct reference between it and the build number. When I installed 0.2 update there was no indication from the install that it had actually took. So was I still running at 0.1?

    Thanks to all for your assistance.
    simonb65 likes this.
  8. simonb65

    simonb65 Alibre Super User

    The build number will always increase on every release, so that's the important bit. Just use that. The build number is what Max and the Alibre team always refer to with any update or comment regarding a fix or known issue it's not meant to signify anything other than one release is after/before another (not all builds are released to customers, some are internal to Alibre or for staged testing). The 2019 bit is important for maintenance. The rest is not really useful in any way shape or form and there isn't any correlation between the 0.2 and build number, it's just an incremental value the developers will use to mark major and minor release chunks!
  9. tk1247

    tk1247 Member

    Yet another example where "snap to feature" capability would be helpful while sketching.
    DaveD44, bigseb and simonb65 like this.
  10. simonb65

    simonb65 Alibre Super User

  11. bigseb

    bigseb Alibre Super User

  12. NateLiqGrav

    NateLiqGrav Alibre Super User

    Inside the sketch you can create a 3d point or axis by going in the menu:
    Sketch > Insert > Point
    Sketch > Insert > Axis
    You can snap to these.
    idslk likes this.
  13. tk1247

    tk1247 Member

    I understand how it can be done as things stand, but that involves unnecessary extra steps. Automatic snap to features like midpoint, intersection, vertex, center, tangent, plane, etc. is a capability that is present in most other CAD systems that really makes sketching faster and easier. When you move your cursor around to place an object, lines will extend automatically to show tangent, perpendicular, and parallel references to the above points, that make initial placement very quick - one can then finish constraining the feature to complete the sketch. Having to execute multiple step constraint operations just to place features is not efficient. I know we could benefit from having that in AD. Just saying..... Still also waiting for a grouping command, as well as a constraint to center an object between two other objects.
    simonb65 likes this.
  14. DaveD44

    DaveD44 Member

    I've been using 2D CAD programs for twenty-something years, starting with AutoCAD Rel. 13, even earlier with some freebies, and later DraftSight, but since Dassault have now priced DraftSight out of my market, NanoCAD 5.0. Entering 2D sketches with all of these products is incredibly easy and there is never an issue with just where a point or intersection is; e.g., zooming all the way in with any of those products returns a display where the lines are well-formed and connections are right on point. The Alibre approach to the 2D sketches has befuddled me from the beginning, but since I'm a newbie with 3D modeling programs and know nothing about the underlying architecture I have mostly kept my silence and tried to learn how to use it productively.

    So I have a question, and it is not of the rhetorical type: In a few words, can anyone tell me just why Alibre doesn't use the tried and true 2D CAD method of making 2D sketches and then add the 3D features--extrusions, lofts, revolves, sweeps, 3D curves, etc.--to these basic 2D drawings. Does the underlying architecture make this impossible, is it simply incompetence, or something else? I settled on Alibre versus other 3D modeling programs and don't have the time, ambition, or money to go looking at other solutions, so question 2: Are all the 3D modeling applications like Alibre in this regard?
  15. simonb65

    simonb65 Alibre Super User

    It does!

    Not sure how you're approaching it, but take a look at the Alibre tutorial.
  16. tk1247

    tk1247 Member

    Don't get me wrong, I really like most of AD's features, like the ability to construct with sketches on surfaces or planes, then constrain and create 3D, and then create assemblies - that is why I picked it. I am simply talking about improving the method of creating sketches, wherever they are, by adding the tried and proven methods of snapping to features. I've seen and used that in TurboCad, Autocad, Rhino3D and others, and it makes sketching SO much easier, as does Grouping for moving etc, and the special constrain of centering objects between other objects (this is simply the mirror opposite of the existing Symmetric Constraint)
    Any comments on those features, Max?
  17. DaveD44

    DaveD44 Member

    Sorry, Simon, but it does not. Please re-read the first paragraph of my post directly above yours and tk1247's comments below yours. It really doesn't come close! Why, if is does, when I created the points on my sketches and "snapped" to them with my loft curve ends, the snap did not take, even when I re-did it directly with a Coincident Constrain? Why then did I have to zoom all the way in, discover the offset, create a reference line from the geometry below, and move the sketch precisely to that location. Why wasn't the curve actually snapped to the point, which was on the corner of my sketch, instead of to some line I could not even see. Too many "whys". And yes, I have reviewed, repeatedly, the tutorials, videos, and the way-back level exercise manual.
  18. idslk

    idslk Alibre Super User

    Hello tk1247,

    these two figures on the sketch are "grouped" (due to the 2 dimensions between them)

    now you can move them together to a new place
    and if you grip the point (red marked) and you drag the point towards the origin, the group will snap to this place...


    and is now automatically fully constrained...

    Last edited: Aug 10, 2019
    Specktech likes this.
  19. simonb65

    simonb65 Alibre Super User

    My comment was a response to your 2nd paragraph, not your first, hence the inclusion of a quote from your post!

    You need to clarify what you actually mean in the second paragraph as I suspect what your thinking is not how it reads. Maybe an example of what steps you would expect to achieve a 3D feature and how Alibre doesn't achive that would be helpful. I've used may 3D CAD packages and Alibre is fairly typical.

    If its specifically how you insert 3D sketches for guide curves, etc. Then I agree Alibre is not the best or most intuitive. 2D sketches are standard across 3D CAD packages.
  20. tk1247

    tk1247 Member

    I think you're missing my point. I acknowledge and understand that there is a way to group via dimensions and constraints, but that it is not the most efficient way when sketching. In the other programs I mentioned, to group things, you just execute a boundary select, click group, then move them around in unison. You can then dimension, constrain, ungroup, as you see fit. These things are sketching tools, not constraining tools, and make the job of sketching easier and less steps. Have you experienced them in other programs? In the programs I mentioned above, if you want to sketch a line between two sides of a rectangle, for instance, if you hover the cursor near one side, the cursor will "snap" to the midpoint, vertex, intersection, center, etc of the side or corner and display a label that you are at the midpoint, vertex etc. It will also project reference lines from the cursor, that move with the cursor, showing perpendicular and horizontal alignment of the cursor to a feature. Again, these are sketching aids, not replacements for constraints. I think they're very desireable, as do, evidently, others, and I'm just lobbying for their consideration for future AD updates.

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