Hi All
I seem to have encountered a frustrating issue when using split body - the faces/edges of a body seems to shift around slightly after a split body command, causing subsequent operations to fail due to the misaligned edges.
Firstly, I confirm that the edges are aligned to begin with:
Very frustrating. I have also tried a number of different methods to create the blend loft, including creating a separate sketch curves, but encountered similar issues, where any tiny, sub-micron misalignment causes errors, or a lack of true tangency.
This method I’ve used should theoretically be the most accurate without a loft feature that allows one to set tangency to neighbouring faces/curves. Also without the ability to create 3D curves, such as bridge curves (I.e. not ones that only sit on a 2D plane) it’s pretty hard to get some things done.
I’m an Siemens NX user of over a decade (which also uses the same Siemens Parasolid engine) so I’m pretty comfortable with how the engine responds to things, but this is a very difficult first-order challenge to overcome
Issue Part.shapr (5.8 MB)
Shapr file to see if the issue can be replicated by others, thanks in advance!
Hi Ben, the good news is that the geometry is actually correct, the bad news is that this is unfortunately an error in how we display mm measurements. In this case 0mm should be displayed. Thanks for reporting it, fix is coming.
I replicated the shapes and there wasn’t really a problem for me:
I think looking at your original, your initial sketch has a very slight offset:
Interesting. Thank you very much for the replies!
Were you able to complete the blend loft between the upper and lower revolves SM1?
SM1 I think you might be right about the sketches, I managed to achieve the desired shape by starting from scratch, then the issue didn’t seem to appear.
I’m wondering if perhaps the issue came from moving the position of the edges or faces around AFTER revolving one of the rings - it might have appear as 0.0000mm but was really 0.0000##mm out…
Thank you for the help so far. I seem to have a slightly different issue now… when trying to import the .shapr file that I uploaded above into the Windows version…
Any idea what could be causing the corruption? It still seems to open fine on the iPad version, Thanks.
Yeah I could loft it
But yeah, sometimes if you don’t have a simple and defined sketch when creating something- it can create small discrepancies that just compound.
Thanks again SM1 
Last one, I promise 
, but were you able to loft it but still maintain a tangent curve on the inner diameter?
I didn’t have an issue with creating it as you have shown, but only when I tried to use the revolve segment as a guide curve did it fall over and give the error…
Anyway I appreciate the help. I will pay extra care with the snapping, using a pencil for modelling is quite alien to me… but liberating!
Hi Ben,
Guided loft requires perfect guides as the tool has no tolerance at all.
In your case, you will need two inner guides if you want to keep the inner circular shape, each guide being perfectly connected to the 3 edges of each face.
To do so, as in the video:
Then, project the top and bottom inner edge of the body you want to substitute to the 2 planes and ensure that each end of each projected curve is connected to the 3 corresponding edges by moving the point and bringing it back to it’s original position: the 3 corresponding edges must highlight. If you don’t do this, it will probably fail.
Then, you will be able to loft, using the 2 guides 
@BenLewisMAV are your running the latest version on Windows?
Thank for you for the video PEC. Yes this is how I managed to get it working - after having to rebuild the model from scratch.
I think the issue I explained/demonstrated in the original post still exists (and repeatable, please try splitting the body and try lofting the ‘Issue Part.shapr’ file above);
The faces appear to be in a certain position (in this case, edges that are ‘0.0000mm’ from each other) are actually not EXACTLY 0mm from each other, as they have been shifted to this position, using the Move command. So when other operations are carried out on them, such as a Split Body command, they behave strangely, moving around slightly, which causes the subsequent Loft command to fail…
I would normally say that this is not much of an issue, as in my typical workflow (Siemens NX), most items are generated and automatically updated from a sketch, so it’s simple, just quickly update the sketch, and the revolves and the rest updates… However with direct modelling, where bodies are not linked/updated from sketches, and users are encouraged to modify and adjust bodies that are already existing (hence, direct modelling), I believe this is quite an issue/challenge to avoid downstream commands failing…
If the method of adjusting faces (move/offset) aren’t robust or accurate enough, then every time I want to adjust a feature that has been lofted and blended, I have to;
(especially vs linked sketches/parametric modelling: 1) update sketch, 2) the rest updates, provided the changes are not too extreme)
I think there needs to either be;
a) A tolerance on features such as loft, to avoid them failing. I’m talking pretty small here, bearing in mind the edges were measuring as 0.0000mm apart before ‘jumping’ apart during the Split Body command. This should be possible using the Siemens Parasolid engine, such as seen on the commands in NX;
b) To have more precise control or snapping when direct modelling adjusting edges or faces using Translate/Move commands. Translate is good, but I have not been able to select centre points on anything but primitive geometry (cylinders, cones, etc.). In this case it is the centre point of the edge/arc that I need to select, so that I can truly align the edges of the green and orange revolves.
Also, having the options of what to snap to during Translate might be quite useful,
like in the sketch environment - but in 3D, after all, modifying 3D geometry is what direct modelling is all about!
Anyway I love the program and continue to use it whenever possible for simpler components/smaller assemblies, please keep updating it. It’s soo close to displacing full-size CAD for component modelling, just still a few frustrations that have meant modelling takes quite a bit longer than necessary.
So, either adding snapping for aligning 3D objects (i.e. a more powerful translate tool, that can snap to; arc centres, midpoints, intersections, quadrants, etc), or a tolerance (say 0.001mm?) on more complex commands like loft would save a huge amount of editing/rebuilding time, and allow direct/synchronous modelling to be a lot more powerful and accurate.
Yes, Istvan, I am. Thank you for the reply
