Reorient alternatives? Or, am I doing it wrong?

[OldDraftsman]

Hi All,

I am still having an issue with the Reorient frequently being grayed out. If I close FC and restart, load the same file at the same point it is no longer grayed out and I can use it for the exact same sketch. Doing some research I hear mention of alternative methods to using reorient. To wit, ChrisB: "It is not clear, what the target is. Usually you don't need to reorient the sketch, you simply attach them to another plane or you modify their AttachmentOffset." https://forum.freecadweb.org/viewtopic. ... 78#p262148

I use Reorient when I need to go back and change stuff that I know would trigger the Topo-naming-crap. I rename ("...-01" etc) the Sketches
Sketch-199-03
Sketch-200-02
Sketch-201-01 <-- last Sketch

Then Reorient to detach from that face in order from the bottom up. I make the changes and then "Map a Sketch to a Face," in the reverse "03, 02" sequence back to where they were and "Pad." (or whatever) This has worked OK until v0.17/v0.18, but now the reorient is often grayed out and restarting FC 20-times is getting tedious.

Is there a better way to do this to skirt around the topo-naming thing? I tried using the approach shown in some of Harry Geier's videos using Datum Planes (https://www.youtube.com/watch?v=YvI_pKohTVc) but that is super cumbersome. It takes a lot of Datum Plane building for something that may never be needed, but, invaluable if it is.

A zillion workarounds should not be the primary method of doing things, Topo needs fixing.

[GeneFC]

This is probably not an "approved" method, but something that often works for me in this situation is to simply detach the sketches and do nothing else. No need to reattach or reorient further. If the sketches are fully constrained and were placed correctly originally they will typically stay put in the original location and they will still work.

Clearly this is a very non-robust process leading to a house of cards. I would only use it if the model is otherwise complete. Always a good idea to have a fresh save to go back to if this trick fails.

Gene

[OldDraftsman]

is to simply detach the sketches and do nothing else.

Thanks for the reply. How do I detach the Sketch? I tried a right click and "Move object to other body," but I get a message "Some of the selected features have dependencies in the source body," and will not allow the move.

Safe-copies? I make them almost by the minute sometimes.

[ppemawm]

I assume that you are using the PartDesign workbench and V0.17 or later.

You can avoid the topo issues by simply attaching the sketches to one of the origin planes or a master sketch and then offsetting and/or rotating the sketch using attachment offset, as required. You can also copy these sketches and change the attachment offset if desired without changing the attachment mode. I never have used Reorient since leaving V0.16.

The downside is that when you create a new sketch you usually have to immediately close it, set the attachment properties, and then reopen the sketch. They are also not parametric in the sense that if you change a feature upstream in the tree you may have to change the attachment offset.

I rarely used datums (sometimes, only if there are multiple sketches at the same location or for 'hard' location planes ) since they duplicate what can be done with the sketch attachment modes.

[HarryGeier]

Frank once described it in depth in his epic videos.
I also do that in some of my videos. I can create a micro tutorial on that matter as ist seems a bit on the dark side.. but it is a very valuable thing..

Select sketch in active body.
Menu Part Design --- reorient Sketch
Confirm detaching from support
END Function, do not reorient NOW
select new plane or face ( baaah.. not good ..but possible )
in Part Design Menu select MAP SKETCH TO FACE
Select the detached sketch

[OldDraftsman]

Thanks Harry and ppemwam:

But that's the point I keep trying to make is, that these things are workarounds for an intrinsic problem that is perpetuated in versions.

I started a thread in the Open Discussion Forum to throw some cash at the devs to try and put a stop to this insanity. The FC is getting feature rich and dragging along a dead horse (Topo-naming) that does not stop stinking -- ever.

In software there should never be a workaround that passes up to the next version. I have been using FC since 0.15 and and with 0.18, that horse still stinks.

[OldDraftsman]

Select sketch in active body.
Confirm detaching from support
END Function, do not reorient NOW
...

Thanks Harry, I assume you mean click "Cancel" in the "Choose orientation" dialog that follows the confirmation. I already do that, but if the sketch is in the middle of 20-others, then is screws up other following stuff big time.

[GeneFC]

Sorry I was not clear. I agree with Harry 100%.

If the following steps are screwed up then this simple fix probably will not work. It works for me quite often, but not always. That is why I highly recommend a "save" before trying the fix.

No disagreement on the toponaming issue, but it appears to be very difficult to solve.

Gene

[NormandC]

This has worked OK until v0.17/v0.18, but now the reorient is often grayed out and restarting FC 20-times is getting tedious.

It happens to me too, but it is not reproducible on demand.

I find that what can help is to switch to the Sketcher workbench, which has the same Reorient sketch command. Then once done, I switch back to PartDesign.

I tried using the approach shown in some of Harry Geier's videos using Datum Planes (https://www.youtube.com/watch?v=YvI_pKohTVc) but that is super cumbersome. It takes a lot of Datum Plane building for something that may never be needed, but, invaluable if it is.

A zillion workarounds should not be the primary method of doing things, Topo needs fixing.

It is not a workaround, it is the proper parametric method, the one that ensures maximum model robustness. And it's true for all parametric, history-based CAD programs.

If you're unwilling to go through this process, then you have no choice but to live with the consequences.

I will add that I work daily with a mid-range commercial CAD program that cost around $12,000CAD a seat about 15 years ago, it does not suffer from the topological naming issue like FreeCAD - yet, I find myself frequently having to delete and recreate external geometry that has lost its link, remapping sketches that have lost their support face, etc. That's because I don't always follow the robust workflow, to save time. For me it's a trade-off, for when I judge it might be quicker repairing an "improperly" built model than to make a robust one. Like it or not, it is the very nature of parametric modelling: its greatest strength is also its greatest weakness.

Solving the topological naming issue in FreeCAD will not be the silver bullet so many of you are expecting.

Here's some very useful reading about another commercial parametric program: https://dezignstuff.com/why-solidworks-needs-a-system/

I've followed Matt Lombard's blog for years because even though I don't use Solidworks, I find his insights often apply to most CAD programs.

Excerpt:

Now we have to talk about Pro/E. Remember Pro/E had a reputation of being difficult to use, and fairly rigid when it came to procedures. Back in the early 90’s, people who taught Pro/E taught some kind of method, or structured procedure. Something like a skeleton model, master model, or references built around planes. It was structured, it was tough to use, people failed to follow the procedures sometimes and made a mess of things. But it worked if you followed the procedure. Models were less likely to lose parent/child relations if you built everything around planes and sketches (like Stoltfus’ SSP method).
(...)
This is the point where all of those people who stopped reading this too-long blog already need to listen extra hard. It turns out that just modeling without any system leads to the chaos that it sounds like it would. There was a reason Pro/E was hard. There was a reason Pro/E users looked derisively down on SW converts. If you have a history-based model with intelligence built in, that intelligence needs to be structured, or it’s just chaos. SolidWorks freed the market by loosening the restraints, damn the chaos. Ease of use as a mantra really gets people’s attention, but discipline is less sexy. Regardless if you do it or not, history-based modeling really needs some structure – rules and procedures.

[OldDraftsman]

It happens to me too, but it is not reproducible on demand.

Well, that is reassuring as I was beginning to wonder if it was something I was doing. But, back in 0.16, I was able to get around with the renaming and reorienting procedure I outlined above. I would sometimes have 6 or 8 hanging sketches to get back to the one I needed to fix. Then I would just go through and reattach and Pad (or whatever). Not a great process but it was fairly quick and easy to do. But, 0.18 is not so generous.

It is not a workaround, it is the proper parametric method, the one that ensures maximum model robustness. And it's true for all parametric, history-based CAD programs.

If you're unwilling to go through this process, then you have no choice but to live with the consequences.

I am happy to try and follow the process, but the current process is not working correctly. As I have previously mentioned, Fusion360 has a time line along the bottom of the screen and I have watched people (youtube) go back and click an icon, make a repair and then carry on. I have no idea if that is using Topological name or or not.

I know next to nothing about programming graphical or CAD stuff, but IMHO, that is how FC should behave and not arbitrarily rename entire sections with the erratic results.