I often have problems with the extrude and offset tools wherein they produce strange lines in the result. These lines seem to have no correspondence to any existing geometry. They simply seem extraneous, and they appear unpredictably. Also, strangely, they can be selected, but not deleted. Can anyone shed some light on what is going on here? I’ve included some screenshots that demonstrate the problem.
In the sketch are the lines transition points in the curve? If they are 2 segments then I can see that happening. If that is the case try selecting both segments and hit the tangent?
Hi, thanks for your response. I’m not sure what you mean by “transition points”. Do you mean the control points of the spline that was used to create the body? If so, then no, the lines do not correspond to the location of the control points. Also, if that were the cause, I would expect to see lines corresponding to all the other control points. If, by “transition points”, you mean places where two curves join, then the answer is also no. There was only one closed spline used to create the body.
I should also mention that, in an effort to reduce the problem, I removed all other geometry from the design. There is only this one body left in this design - no other bodies or sketches.
I simply meant separate line segments. IIRC this subject has been in the forum before with no solution.
Thanks Oregonerd. I looked before posting, but didn’t find the thread. Maybe I don’t know what the right name for this problem is. Let’s hope there’s a response from the Shapr team.
One more thing. Are the there 2 bodies or 1?
There is only 1 body. I am extruding it to create a second. (although the same lines appear if choose “union” rather then “new body” in the options.
Oregonerd’s opinion was right, the curves are placed in the transition point of the contour, this is the point where the curvature changes direction.
As I see, you are using the Extrude command. I guess your goal was to make a new body on top of the existing one, otherwise, the simple Offset Face tool would be fine. When you have decided to extrude the grey body, Shapr3D grabbed the contour of the bronze one and extruded as a grey body. The contour has the same shape as the bronze one’s, but mathematically (control-point wise) may differ. This is why you have an edge at the transition point. It can be selected and moved, but it cannot be deleted. It is not a sketch, it is a part of the solid body.
To avoid those edges, you can do two things:
Use the sketch of the bronze body, extrude a new body with the thickness of the grey one and move it up
Use the Offset Face tool, then select a side view, draw a rectangle that covers the grey part of the body. Extrude the rectangle into the body as a new body and find the intersection of the rectangle and the original body. Now you have the upper part, which have to be Subtracted from the bottom one with keeping the originals.
If I ended up confusing, please let me know and I will make a video
Thank you for your response, and for trying to explain what is happening here. I still have have a few questions.
I would like to understand what a “transition point” is. The original curve that created the bronze body was created with a single control spline. It began and ended at a single point. Is this what you mean by a “transition point”? If so, why is the original body smooth and free of lines that represent this “transition point”? Does that mean that the original curve has no transition points?
I have tried selecting and moving the lines as you suggested. They can not be moved. Also, any attempt to push or pull on them with the chamfer/fillet tool results in the error “failed to compute geometry”. If these lines do not represent an actual edge in the model, and can not be moved or manipulated in any way, then why are they being displayed to the user? What do they represent?
Why would the curve of the extruded body be mathematically different from the original? What is causing it to be mathematically different (producing lines) when using the extrude tool, but not mathematically different (no lines) when using the offset tool?
Is there a reason that the user would want a result body from the extrude tool that contains these lines? Is there a reason that the user would want such lines from the extrude tool, but not the offset tool? If not, can you perhaps acknowledge that this behavior is unintentional, confusing to the user, and needs a remedy?
Thanks for your attention to this.
I’m curious, that maybe the lines appear when extruding because extrude also can produce a draft angle, and those edges are produced because of that, even if no draft angle is specified.
Offset face doesn’t option a draft angle, and there are no lines.
This is just a theory.
On Q1: Even though you used a single spline, that spline is a series of curves. Math formulas describe those curves (Vectors). Where one curve ends and one begins is the transition. Lookup Quadratics and curve plotting to see how curves are graphed that will give a clue to transitions I meant.
I worked as a rear chainman on a surveying crew in my youth (Rear Chainman = Dummy on the stupid end of the tape measure.). Plotting curves in roads, fun stuff!
I hated Quadratic formulas until I was told what they were used for. No graph plotting calcs back then (that one could afford).
Q2-4: This has been asked more or less before, How do they affect the project other than visually is the concern. Computing the chamfer is one way like you are experiencing. I am having that problem my own self on a project extruding text.
Hi Oregonerd. Thanks again.
I hear what you are saying about a spline being a series of curves. If what you are saying about the lines representing underlying transition points, then my question to the Shapr team is why are they sometimes displayed, and others not? Why the inconsistency and unpredictability? Presumably, it not functional that these lines show up unpredictably. This suggests a bug somewhere, one that I am requesting and hoping that they fix.
I would also say that it is more problematic than an aesthetic issue. It is confusing to the user to be presented with lines that suggest edges in places where they are not expected or desired, and that these edges are somehow different from normal edges which can be manipulated. In addition to being visually confusing, which slows down work flow, it suggests to the user that they have done something wrong, or that the model is broken in some way that needs fixing. It causes the user to waste time trying to fix the model in futility.
Thanks again for trying to sort me out. Let’s hope that Shapr team acknowledges that something needs fixing here.
By transition point I meant the inflection point, where the curvature changes it’s direction. The original spline that defines the bronze shape was one piece of spline, but when you started the Extrude tool and selected the upper surface, the edge of the surface got kinda projected. Altough it has the same shape as your spline, it differs from it because it is a result of an algorithmic process. It probably has more control points than the spline you made and it may made up from more than one spline elements. Where these more than one elements connect to each other, you will see that edge. They are usually at the inflexion or quadrant points of the curve and in detailed surface modeling they are really helpful references for connecting surfaces. In Shapr3D - currently - they are the displayed results of the computational process made by the modeling engine Shapr3D uses.
I am sure that if you translate the original spline to the upper edge of the bronze body (even with copy on) and extrude the enclosed area of the curve instead of the upper face of the bronze body, you will have no edges there
By simply selecting an edge with the pencil you will be given the Chamfer/Fillet tool automatically, which in this case will fail to compute geometry. By selecting the edge and trying to fillet/chamfer it, you are asking Shapr3D to add a fillet or chamfer to an edge which connects two faces that matched by tangent continuity. You cannot fillet the edge, because at the edge of the two connecting surfaces tangent relation means that the radius is infinite.
If the Move/Rotate tool from the Transform toolbar is activated, the edge can be interacted. Which in this case will not be super useful.
The curve is different, because it is not the same curve that was defined by your control points. It is an algorythmic result of an edge duplication made by far different criterias than any geometry placed by the user.
There are many cases when these lines can be useful in more complex modeling. Please note that extruding a surface is totally different than offseting a surface. It may end up in the same result, but these are two different commands.
I hope that one of my solutions above can be useful for you to avoid these edges
All in all I am sorry to see that these edges are bothering you. Believe me, these are not bugs or issues, they are common in the world of CAD software.