Can't get my model to behave parametrically

[kkessler]

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

I decided to try out FreeCad after being mocked by an engineering student for still using OpenScad. So I designed the attached part, exported to STL and printed it, and everything was awesome. Looking at the part, I noticed I had to make "Pad" 5mm instead of 9mm, so I made the changed, and everything went to hell. Fillets appeared out of nowhere and the existing ones got boned up, sketches became invalid and I had to go in to some fix screen and remove external constraints, which did those sketches no good, and, in general, things just fell apart.

I must be missing some basic concepts which allows successful changing of parameters after the model is complete, but I don't even know what I might google? None of the tutorials I've found actually go into changing a model after you've completed it.

If someone could point me in the right direction, I would appreciate it.

[Willem]

Hi, welcome to the Freecad forum, at first I must say that Openscad is a very good program and if you feel comfortable with it keep on using if. Freecad however has a lot of workbenches and that is for a lot user an advantage. The cause of the problem with changing the Pocketdepth from 9 to 5 mm is in the use of the "Create an edge linked to an external geometry" in almost every sketch. Use it only when you can not constrain the sketch with dimensions.
In a reworked model without the external links you can change all dimensions without problems

Another point is you can select more than one vertices for a fillet, when I have to do a lot fillets of the same size I prefer the fillet in the Part workbench above the Part design fillet because this has a menu for selecting and deselecting

[CADinBoots]

EDIT: The above post was not there when I first started this post...

I'm just a noob but the same thing happens when I try with your model.

When you change the pad depth it breaks the sketch for your hole. And if you fix the sketch for the hole by mapping it to the new moved face the sketch goes bonkers because you have to delete the ties to the reference geometries. (The sketch becomes angry and it says you need to fix the sketch to edit it and only by deleting all references can I re-edit).

Then it seems like all the edge names become randomized and you fillet random things. Random fillets thereby break because the random things that get selected to be filleted don't always work.

I confirmed this by replacing the partDesign fillets with a part fillet and the fillet will continue to say, fillet edge 87 before and after changing the pad from 9mm to 5mm... but the problem is that edge 87 is now a different edge than it used to be.

Chaos ensues.

Anyway, the only way I can figure out how to do it is to reapply the fillets and remap the sketches, which may require reconstraining. I reattached the part with a 5mm pad instead of a 9mm pad.

EDITED: Willem appears to have written a better answer, which I will study... I was studying your sketch for the last hour or so with a reply window up, so that's why my reply appeared after his... not time wasted at all for me because I learned a lot trying to muss with it all.

RE-EDIT: It does indeed appear that as long as there are no ties to previous geometries in the sketch that it will allow parametric readjustment on the fly. On Willems (and mine where I inadvertently broke the ties in the name of just fixing the sketches) it allows for a paramteric readjustment now without changing the fillets again.

[chrisb]

Usage of expressions instead of external geometry makes a module very robust. It is not quite as comfortable as external geometry but yet very powerful.

Let's assume this cube, where I want to pocket something from the right upper corner. No problem with external geometry but is easy to achieve with expressions as well:
In the base Sketch I have given a name to the dimension defining the position of the corner. In the Sketch001 I use this dimension. Click the tiny blue icon in the input field and enter the expression in the form SKETCHNAME.Constraints.yourContraintName.
If you dont have the constraint "natuarally" you can add a driven constraint (the blue ones).