Broke my filliter??

[Mongrel_Shark]

HI everyone.

This is my first post here. Been lurking and FreeCADing for a while. So far managed not to break stuff. I'm still a n00bly beginner though.

I seem to have broken my fillet and chamfer tools??

I made some fishing lures to 3d print. Starting with a rectangle then pocketing it to get a taper at one end, then did some fillets etc and it was all good.
Got exactly what I wanted.

Then I tried to repeat the process with some different dimensions and now it wont fillet or chamfer the way it did.
Thought it could be my dimensions so tried to repeat the original sucsessful design. Now that wont work either.

Any ideas?

Here is my version details
OS: Ubuntu 14.04.5 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

I'm a bit of a linux dummy so something is probably out of date. Have a different version on my laptop and I can't do much with it so reluctant to make changes. This version works for me so hoping to stick with it till I get better at freecad....


The 2 files attached with MK1 titles are the ones that worked.
The base is one of the attempts that wont fillet. Every time I try it comes up with errors on the fillet and makes the unchanged part invisible. Like in the attached badfillet file, which is just the base file with broken fillets applied.
I have tried a wide range of fillet radius values. It just wont work again. Even if I try to duplicate the original working model. Having some success with chamfers but they seem to be on the blink too.

Did I do something different in my sketches that’s stopping it working? I feel like I got more efficient with constraints with every new model. Maybe I did something that doesn't get along with the fillet tool?
Or have I somehow broken something?
Tried rebooting computer etc etc. Still wont work. I'm all out of obvious stiff to try.

[Willem]

Hi Mongrel_Shark welcome to the forum. I downloaded your files and after investigating, rebuilding and also rebuilding them in different ways in the part workbench I could not find a reason why the fillet does not work. With my experiences they also failed. I am very surprised that your other files with an identical way of building the design are good. The only way I could succeed is making the design in the part workbench and not in the part design workbench, so I do not know what is wrong in your file but I succeeded in making a design with a good result

[NormandC]

Hello Mongrel_Shark,

Welcome to the forum.

I'm a bit of a linux dummy so something is probably out of date. Have a different version on my laptop and I can't do much with it so reluctant to make changes.

The version you posted is the last release available for Ubuntu on the FreeCAD PPA repository. It is missing 3 bug fixes, the last updated release on Windows and Mac is 0.16.6706. We plan on updating the PPA as soon as possible, when we do you'll get it through the system updates.

As for your laptop, did you install FreeCAD from the Ubuntu repositories? The reason we created the FreeCAD PPA (I was the one who proposed it years ago, got help from one of the FreeCAD devs wmayer to set it up, then managed it until last year when sgrogan took up the mantle) is the the version proposed in the Ubuntu repositories is always outdated, and is often buggy. One notable exception is Ubuntu 16.10 just released, it's got 0.16 but it's missing the freecad-doc package. I'm guessing we'll have to provide it on our PPA as well.

I am as puzzled by this problem as Willem. I couldn't get the fillet to work either, even on a model built from scratch in PartDesign. I am wondering how you managed to make it work the first time. Did you create it in an older FreeCAD version? (I'm on the exact same Ubuntu and FreeCAD versions as you)

The only way I could succeed is making the design in the part workbench and not in the part design workbench, so I do not know what is wrong in your file but I succeeded in making a design with a good result

Just FYI, you can create the main body in one go with a Part Loft of three sketches and the "Ruled" option set to true.

The problem with a shape created with Loft is the the fillet propagates to the next edges even if you don't select them, as your file shows. But in Mongrel_Shark's working model, the fillet is different between the slanted edges (radius of 4 mm) and the straight ones (radius of 2 mm). What's more puzzling, fillets should propagate to the next edges only when they are tangent, which is not the case here.

Very strange indeed.

EDIT: there's another problem with using a Part Loft. The generated faces between the sketches are not considered planar (even if they really are), but as BSpline surfaces. The result is that it is not possible to map sketches to them.

[NormandC]

This is the only way I found that would work.

But doing a fillet on the edges in the middle of the part (where the planes change direction) fails.

I'm starting to wonder if the problem is with the OCC version we're using (6.8.0). I'd be curious to see if there are such problems with older and younger versions.

[chrisb]

Same problem with OCC 7.0.0

OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.8443 (Git)
Build type: Release
Branch: (detached from afa3784)
Hash: afa37847b5082a3677a33809be0f950cfd8d5647
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 3.1.3
OCC version: 7.0.0

[NormandC]

Thanks Chris.

I found a workaround which allows further filleting: create the base solid using a Part Sweep. The trick is to include the 4mm and 2mm fillets in the sketches themselves.

Basically, fillets are a PITA in FreeCAD because of the OCC kernel (it's responsible for all geometric operations). OCC being a third-party library, there isn't much the FreeCAD devs can do about it but hope newer versions fix such geometry bugs. When fillet problems happen, I try to integrate fillets in the sketches, which is what I did here.

Using a Part Sweep with a straight path gives the same solid as a Loft like in my previous file, the advantage over the Part Loft is that the resulting faces between the sweep profiles are planar, so we can map sketches to them.

My file is loosely based on MK1popnose.FCStd's dimensions, but it does not include all the details. I recommend that you apply the fillets to your design as late as possible, in other words when no other feature is needed. In general it is a bad idea to construct sketches over Part or PartDesign fillet features because it makes the model more fragile to changes. In 0.16, when a fillet fails after a change "upstream" in the history if the model, there is usually no choice but to delete it and create a new one.

FC_MongrelShark_base_01.gif (34.17 KiB) Viewed 1089 times

FC_MongrelShark_base_05.png (17.15 KiB) Viewed 1089 times

[Mongrel_Shark]

I recommend that you apply the fillets to your design as late as possible, in other words when no other feature is needed. In general it is a bad idea to construct sketches over Part or PartDesign fillet features because it makes the model more fragile to changes. In 0.16, when a fillet fails after a change "upstream" in the history if the model, there is usually no choice but to delete it and create a new one.

I found that too. lol. I'm good at learning the hard way Except a lot of the time when I delete the fillets and make changes the fillets dont work as predicted the second time around, or they fill pockets back up

Obviously I need to approach it a new way

I'll have to investigate this Part Sweep feature. Any good tutorials I can look at for that?
I'm also curious about the Draft tool in part design. Except I have no idea how to get it to work... I don't think its th right tool for this design, but I have a few variations on this plan where it could be good.

So far I have mostly been working in the part design workbench, where I am starting to get comfortable and even a little fluent, using a few keyboard shortcuts etc.

Done a little drafting on the Daft workbench. Mostly script for pocketing text via boolean cut Which is also a bit buggy, but I see that a well known issue. Also just discoverd the mirror tool. Which saves a lot of time when making left and right wings for a glider lol. First three times I actually made them individually


P.s. I'll go uninstall the ubuntu version of freecad on the laptop and get the PPA

[Mongrel_Shark]

Trying to muddle my way through the part sweep by copying Normans file.

Cant seem to get the circle (made from 4 arcs that’s a neat trick took me a moment to see whats going on there) to go on the end of the sweep direction line.

Am I doing my sketches in the wrong order?

[Mongrel_Shark]

Ohhhh
Worked it out. Offset sketch

I got the tapered part. Now I just need to box out the back half |

Give me another few min... I'll work it out shortly

(scrolls down on this page and looks at gif again)

Oh I see. Thats what that pocket is for .lol.

Ok I'll try that and see what I get with my new version.

[NormandC]

Cant seem to get the circle (made from 4 arcs that’s a neat trick took me a moment to see whats going on there)

Not a circle made of 4 arcs. A square with filleted corners. The line length left is only 0.01mm. Goal is to have the same number of segments between both sketches. Otherwise you don't get a proper sweep.

Oh I see. Thats what that pocket is for .lol.

Or you could just download my FreeCAD file and examine it!