Can't fully constrain sketch Nor find broken portion in order to pad

Post here for help on using FreeCAD's graphical user interface (GUI).
jjman6
Posts: 5
Joined: Tue Jul 26, 2016 8:16 am
Location: Washington State

Can't fully constrain sketch Nor find broken portion in order to pad

Postby jjman6 » Tue Jul 26, 2016 8:34 am

I'm having a multitude of issues.
Aside from the constant crashing of freecad :evil:

So i have reworked this sketch forever. i have moved every single point a dozen times and made sure EVERYTHING won't move. I have spent HOURS & HOURS trying to get this thing fully constrained to no avail. I had it fully contrained at one point but had to go and and delete a bunch of lines that it wouldn't allow me to Trim for whatever reason (and then redraw them only where needed)

But i'm still falling short of 3 degree's of freedom. But even b4 that i had the sketch fully constrained at one point but i still was unable to pad it because it was not a solid. Was getting the error that said it had broken face. But i simply can't find any break anywhere.

I need to pad/extrude this sketch but its refusing to work.

I have zoomed every point on exterior, I have moved every single constraint multiple times(after i find 1 more degree of freedom).

One thing that i'm not sure if its giving me issues or not. But i have created construction lines on the perimeter and i have then redrawn/traced over them as my actual exterior perimeter. So i noticed that i'm unable to HIDE the construction lines so that i can see or even move/constrain or manipulate in anyway the actual lines that lay on top of (or in actual use below, because any selection of the the lines defaults to the construction lines not the drawn lines).

Lastly i was wondering if my arc's were causing the problem of the broken surface. One thing i notice is that while editing the sketch the arc's look fine but as soon as you close the sketch and look at it normally the arcs turn into straight lines. They aren't arcs. they display as arcs in edit. but they are just straight lines outside of edit.

Tried to include as much info as i could. I'm at my wits end w/ Freecad. But there aren't many alternatives in the linux world. Drawings that take minutes in Trimble Sketchup are taking me days and days here and things just keep crashing or failing. I get errors in the Report window all the time on actions i try to do.

There are a lot of constraints in there. as there are a lot of lines.

Here's my info:
OS: Ubuntu 15.10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.10
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17


Here's a copy of the sketch w/ its dependancies.
Sketch name: "ridge"
Attachments
BrokenRidgeSketch.fcstd
Ridge sketch has broken surface and can't fully constrain.
(42.66 KiB) Downloaded 28 times
triplus
Posts: 7927
Joined: Mon Dec 12, 2011 4:45 pm

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby triplus » Tue Jul 26, 2016 2:00 pm

Hi @jjman6.

There are multiple things to improve first.

Remove the tangent constraints between lines and instead use construction geometry:

http://www.freecadweb.org/wiki/index.ph ... uctionMode

Use coincident constraints between line edges instead of fix a point onto a object. Some places to replace:
Coincident.png
Coincident.png (3.41 KiB) Viewed 1286 times
You try to construct sketcher geometry that can't work:
Geometry.png
Geometry.png (3.3 KiB) Viewed 1286 times
Use arc instead of full circle to crate valid geometry for after adding features like Pad/Pocket.

And in general you could Pad the base and after add Pocket for one half and use Mirror feature on it. That would reduce complexity of your sketch in half.
User avatar
quick61
Posts: 3673
Joined: Sat Aug 24, 2013 2:49 am
Location: u.S.A.

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby quick61 » Tue Jul 26, 2016 2:53 pm

Another thing with complex sketches like this, after taking Jim's suggestion to only do half and mirror, when starting the Sketch, start out with one closed profile and fully constrain it before starting to add more lines/arcs, etc.. This will help remove a massive amount of confusion in your construction of the sketch.

For instance, I would start with the lower corner like so -
ConstrainInSteps1.png
ConstrainInSteps1.png (15.57 KiB) Viewed 1276 times
Then add another closed profile and fully constrain -
ConstrainInSteps2.png
ConstrainInSteps2.png (18.82 KiB) Viewed 1276 times
- and one by one add a closed profile, fully, constrain, then do the next one by one and build it up like so -
ConstrainInSteps3.png
ConstrainInSteps3.png (26.46 KiB) Viewed 1276 times
Notice that I do not need near as much external geometry and only a few distance constraints. I'll take it you end result is desired to be looking something like this -
ConstrainInSteps4.png
ConstrainInSteps4.png (5.82 KiB) Viewed 1276 times
The Sketch around the outside is completely unnecessary and will not work when you try to Pocket. Just lay out your pockets on half the shape and then add a Mirror feature as Jim suggests.

Mark
This post made with 0.0% Micro$oft products - GOT LINUX?
jmaustpc
Posts: 8827
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby jmaustpc » Tue Jul 26, 2016 3:15 pm

jjman6 wrote:Aside from the constant crashing of freecad :evil:
FreeCAD should not be constantly crashing. If you can provide a demo file and exact step by step instructions on how to repeatedly get a crash, then please do so. If you are getting a lot of random crashes I would suspect your computer, if its only FreeCAD then my first guess would be because it is pushing your GPU harder or in different ways that other applications. This happened to me once due to a GPU fan being choked with dust and also another time due to dust in the CPU fan which had clogged a filter such that it blocked airflow from the CPU fan.
User avatar
NormandC
Posts: 17791
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby NormandC » Tue Jul 26, 2016 6:48 pm

jjman6 wrote:So i have reworked this sketch forever.
jjman6 wrote: I have spent HOURS & HOURS trying to get this thing fully constrained to no avail.
And yet this is the first time you come here.

Edit: I just realized you are probably the one who was reflecting on #freecad 10 days ago that nobody who was logged in actually monitored the questions. I wrote to you privately but you were AFK. Quite ironic. ;)
jjman6 wrote:I need to pad/extrude this sketch but its refusing to work.
Well you obviously don't understand what it takes to get a valid sketch for padding/extruding a solid, as triplus has shown in the following screen shot.
Image

Instead of persisting in doing everything by yourself for all those hours and getting frustrated, if you'd have come for help sooner, you would not have wasted your time. You are really the only one to blame here.

EDIT: I just had a better look at the model. It's not complete, there's a whole chunk of history missing. The point is, instead of reproducing the complete outline of the part, adding inner profiles then padding to get your ridges, it would have been a lot more efficient to make a thicker pad from the start, then pocketing the inner profiles, kind of what Mark (quick61) implies in his captures. I would also use PartDesign LinearPattern instead of creating repeated geometry in a single sketch.
jjman6 wrote:Here's my info:
OS: Ubuntu 15.10
FYI Ubuntu 15.10 will stop being maintained by Canonical in 2 days, on July 28th. Consequently future versions of FreeCAD will not be provided for it. If you don't want to upgrade your Ubuntu every 9 months, I suggest you stick with LTS releases. That's what I've been doing for the past 4 years.
Last edited by NormandC on Tue Jul 26, 2016 10:36 pm, edited 1 time in total.
User avatar
NormandC
Posts: 17791
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby NormandC » Tue Jul 26, 2016 10:00 pm

Here's a "quick" example applying what has been said here.

It is not complete, but it has taken me less than 45 minutes overall. Much less than your "HOURS & HOURS".
FC_jjman6_model_01.png
FC_jjman6_model_01.png (14.51 KiB) Viewed 1230 times
Basically:
  • Do not try to cram everything into a single sketch. It will take forever to constrain. At 276 constraints and 3 DOFs left, your Ridge sketch is ridiculously complex. I use a parametric CAD system everyday for work and I NEVER sketch anything as complex for such a use.
  • Do not add fillets to your sketch unless they are part of the design. Since the "arms" of the body have holes concentric to the rounded corners, I left those in the sketch. I removed all the other fillets. They should be applied at the end of the modelling process, not before. This simplifies sketches.
  • Use 3D functions to mirror and pattern 3D functions. Look at my Pocket001, and at the PartDesign LinearPattern. In the sketch, I used a construction line and added a reference dimension (in blue). The construction line is used to set the direction of the linear pattern; the reference dimension value is used as expression for the linear pattern length (click on the f(x) icon to see the expression). I could have simply noted the dimension value and input it manually, but I was feeling fancy. :D
Once I judged the half-body "complete", I made a Part Mirror then a Part Fuse to join the two halves. Next I created an OpenSCAD RefineShapeFeature to clean up the solid of residual edges. And only then did I apply PartDesign Fillets.

But please note this is an incomplete example, and I made a mistake in the Ridge001 sketch under the first Pocket. I shouldn't have left the circle there, because a new one will be needed to cut through the whole solid. Best would have been to wait until all the ridges were pocketed to pocket the end hole, the other whole on the main body and the half-slot, before mirroring the body. My model is also missing the "fin" at the rear of the body.

Version used:
OS: Ubuntu 14.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-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
Attachments
jjman6_model_normandc1.fcstd
(157.37 KiB) Downloaded 19 times
User avatar
NormandC
Posts: 17791
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby NormandC » Tue Jul 26, 2016 10:26 pm

triplus wrote:Remove the tangent constraints between lines and instead use construction geometry:

http://www.freecadweb.org/wiki/index.ph ... uctionMode

Use coincident constraints between line edges instead of fix a point onto a object.
I don't know if that was jjman6's intention or if it was a mistake, but I profusely use a point on object constraint to align lines with each other. I find it faster than using a small construction line between say two rectangles.

So instead of this:
FC_aligned_lines_01.png
FC_aligned_lines_01.png (5.3 KiB) Viewed 1225 times
I prefer to do this:
FC_aligned_lines_02.png
Select one line on a rectangle, and one point on the other...
FC_aligned_lines_02.png (4.59 KiB) Viewed 1225 times
Then I add a Image point on object constraint.
FC_aligned_lines_03.png
...Create a point on object constraint.
FC_aligned_lines_03.png (4.47 KiB) Viewed 1225 times
Of course, the advantage of using small construction lines is that you can set an equal length constraint between them and add a single dimensional constraint to set the distance between profiles. I didn't bother to do this in the example file I posted previously. Call me lazy. :D
triplus
Posts: 7927
Joined: Mon Dec 12, 2011 4:45 pm

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby triplus » Tue Jul 26, 2016 11:05 pm

NormandC wrote:I prefer to do this:
Nice tip.
I don't know if that was jjman6's intention or if it was a mistake, but I profusely use a point on object constraint to align lines with each other.
In the places i added blue dots on the image above i guess it was assumed fix a point onto constraint should do the job. If my check was correct at least one additional constraint is missing for each.
Call me lazy. :D
Lazy.

P.S. Although you spend too much time on it and i don't feel it's fair.
jjman6
Posts: 5
Joined: Tue Jul 26, 2016 8:16 am
Location: Washington State

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby jjman6 » Wed Jul 27, 2016 4:39 am

Just want to say THANK you so much. You guys have given me a ton to process. Yes i'm still learning freecad.

Normandc yea u nailed that's what i'm going for.

I had it fully constrained initially but then realized i had to trim all the connecting lines. at which point i started doing that (several that i couldn't trim, probably because of not know exactly how the trim tool functions) But i was forced to delete lines and redraw the individual segments.

So i went from a fully constrained (but still somehow broken surface) to a 40+ degree's of freedom. And proceeded to try and fully constrain it again. Also it wasn't quite as complicated initially when i had first had it fully constrained but as i had to remove a lot of the longer lines and break them into individual sections. it got a lot more complicated w/ a lot more constraints to deal with.

I will pour over all of the feedback more thoroughly later when i have a chance to actually work on the drawing.

And in regard to not seeking help sooner. #1 Yes i was the one on the IRC over a week & getting no responses or help. #2 i try not to bother ppl with help until i have exhausted my inability to figure it out. As my experience with asking for help online is well; "RTFM is the general demeanor". I have come a lot further in the few weeks i've been using freecad tho.

Anyway thanks,

I'll check back in after i reviewed all the responses, that frankly i didn't expect to get so quick nor so thorough here :shock:

And yes i will be upgrading my Kubuntu to latest LTS very soon. I have just been procrastinating that inevitability.
User avatar
NormandC
Posts: 17791
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Can't fully constrain sketch Nor find broken portion in order to pad

Postby NormandC » Wed Jul 27, 2016 6:20 am

jjman6 wrote:#1 Yes i was the one on the IRC over a week & getting no responses or help.
jjman6 wrote:frankly i didn't expect to get so quick nor so thorough here :shock:
I engaged a private conversation with you on the #freecad IRC channel, but you weren't replying so I left after a few minutes. I seldom use IRC so I have no idea if the conversation was deleted when I logged out.

If you did read my comments, well duh! I did say that *the* place to get quick and efficient help is right here, period. :D Not on that #freecad wasteland. Sure you got a couple of devs discussing over there and occasionally an end user or two, but all the FreeCAD developers and all the experienced FreeCAD users are active on this forum, not on #freecad.

I read almost daily the IRC logs on http://freecadlog.archivist.info and I really can't believe the people who persist in hanging out on that channel, asking for help on FreeCAD use, getting no answers yet coming back day after day... It's baffling to witness. :shock:

IRC is such an obsolete medium, utterly unsuited for getting help on a program like FreeCAD. This forum allows us to attach images and FreeCAD files (even DXF and others), conversations are separated by topics archived for posterity, replies to a question can be very thorough, well formatted, etc. What's ironic is that web-based forums have been around for more than 15 years. phpBB, the forum engine used here has not changed much since. I'm not on Facebook but I frequent Google+, I moderate the FreeCAD community over there, and frankly it is much easier to communicate on this forum than on G+.
jjman6 wrote: As my experience with asking for help online is well; "RTFM is the general demeanor".
Point well taken, many of us (and that includes myself :oops: ) in open source communities have this habit. Truth is, relating to the FreeCAD project, there's not many people who work on documentation, and with FreeCAD's development cycle it's difficult to keep up. So the forum is here to fill in the gaps.

Also you might be interested in the new FreeCAD manual.
triplus wrote:Nice tip.
I'm sure you know that the tangent constraint can be used to make two lines collinear, but after experimenting with the feature I found that it was introducing instability to the solver, with the geometry locking up at some point like jjman6 was seeing in his sketch. So I stopped using the tangent constraint that way. But that was a couple years ago, maybe things have improved since then.

And I'm now one reply short of 10,000. :ugeek: :mrgreen: