Removing splitter failed

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Barnaby
Posts: 3
Joined: Sun Mar 19, 2017 5:03 pm

Removing splitter failed

Postby Barnaby » Sun Mar 19, 2017 5:20 pm

OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: tag: 0.16.6706
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.11
Qt version: 4.8.7
Coin version: 3.1.3
OCC version: 6.8.0.oce-0.17


Hello,

I’m following the following tutorial: http://freecad-tutorial.blogspot.co.uk/ ... iston.html

And I’m trying to pad the parallel walls of the cylinder head but I get an error message “Removing splitter failed” if I enter the 48mm (reversed) pad dimension. I can do the pad in the positive direction, but strangely to me, I can also do the pad at a 85mm (reversed) i.e. going beyond my desired dimension.

I've attached the drawing as far as I've got if that's of any help.

I’m very new to FreeCAD and have been working my way though tutorials, but this pad behavior seems odd, if it totally failed I’d assume it was an issue with my sketch, but it seems to work for particular pad lengths and not others.

Can anyone tell me where I went wrong? Many thanks, Barnaby
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chrisb
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Joined: Tue Mar 17, 2015 9:14 am

Re: Removing splitter failed

Postby chrisb » Sun Mar 19, 2017 6:56 pm

Although I haven't seen this problem in connection with Part Design Workbench it seems like the problem with the coplanar faces. If you change the pad's type to "Two dimensions" and make the first length 0.001 mm it works with 48 mm to the other side.
Barnaby
Posts: 3
Joined: Sun Mar 19, 2017 5:03 pm

Re: Removing splitter failed

Postby Barnaby » Sun Mar 19, 2017 7:10 pm

Thank you Chris, that's great I can now continue with the tutorial.

I don't profess to understanding why that works, but appreciate sometimes you need to nudge things in the right direction.

All the best, Barnaby
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NormandC
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Location: Québec, Canada

Re: Removing splitter failed

Postby NormandC » Sun Mar 19, 2017 7:19 pm

Hello Barnaby,

Welcome to the FreeCAD forum.

Barnaby wrote:I get an error message “Removing splitter failed”

This is a message from the RemoveSplitter() algorithm that cleans up faces of the residual edges left by Boolean or feature-based operations. This algorithm is implemented in the GUI in 3 different ways: from the Part --> Refine shape menu (creates a new unlinked object, thus should only be used on converted meshes or imported solids), the OpenSCAD Refine Shape Feature and an automatic mode in the preferences.

Therefore, you are getting this message because you enabled "Automatically refine shape after Boolean/feature-based operations" options in Edit --> Preferences / Part Design / General. This message is telling you the algorithm has failed to operate and prevents the Pad from completing.

You can avoid this message by deactivating the auto refine settings then editing the Pad again. But know that doing so in the middle of a model can be extremely disruptive. Your model only contains 2 sketches and 2 features, the results are fine. But doing so on a model with many features and sketches would be catastrophic and break the model. For this reason, even if the auto refine options were implemented on my request, I no longer use them for files shared in the forum. I prefer to use an OpenSCAD Refine Shape Feature once the model is finished.

That being said, it is always best to avoid tangent and coplanar surfaces when applying Boolean operations and PartDesign features.

The problem you are having can be fixed in a cleaner manner if you edit Sketch001 and change the radii values from 37.5mm to a smaller value, for example 37mm. This way, the produced pad will have a smaller diameter than the outer body, this will fix the remove splitter error and you'll be able to pad to exactly 48.000mm.
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NormandC
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Re: Removing splitter failed

Postby NormandC » Sun Mar 19, 2017 7:25 pm

One other thing :)

You can do your Sketch001 more efficiently:

  • Rather than set two radius constraints, you need only create one, then apply an equal length constraint between the two arcs
  • Rather than setting two 30mm horizontal distance constraints for the vertical lines, you need only create one, then apply an equal length constraint between the two lines.
It is always best to limit the use of dimensional constraints, and prioritize geometric constraints whenever possible, because dimensional constraints are more taxing on the Sketcher solver. Another advantage is that if you need to change either the radius or the length of the lines, you only have one value to edit instead of two.
Barnaby
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Joined: Sun Mar 19, 2017 5:03 pm

Re: Removing splitter failed

Postby Barnaby » Sun Mar 19, 2017 8:12 pm

Hi NormandC,

Thank you for the explanation, I enabled the "Automatically refine shape after Boolean/feature-based operations" feature as part of another tutorial series I was following on youtube. I'll go back and turn it off now.

I appreciate you looking at my sketch and seeing how I could be more efficient, following your suggestion I did the next sketch with three dimensional constraints and the rest were geometric. It's going to take a bit of practice to learn how to efficiently constrain the sketch, but at least I'm beginning to get a glimmer of understanding. :?

Thanks again, Barnaby
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NormandC
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Location: Québec, Canada

Re: Removing splitter failed

Postby NormandC » Sun Mar 19, 2017 8:19 pm

Hello Barnaby,

Barnaby wrote:It's going to take a bit of practice to learn how to efficiently constrain the sketch

It sure will! :D

I'm afraid this is the kind of thing that you get through practice. I was introduced to the concept of constraint-based sketching back in 1998 :? , but only started working daily with such a system (on a commercial CAD program) 10 years ago. Still, sticking around this forum and testing FreeCAD and helping newcomers learn it helped me learn yet more stuff about sketching with constraints, and I use this knowledge learned in FreeCAD in my daily job. :)

Cheers,

Norm