New user observations & guidance request

[GeneFC]

I believe your strategy is very difficult at best.

Your model delta28BYJ-bracket04.fcstd has way too many bodies, several of which are empty. Yet it appears that you are trying to make a single solid object. Also, mixing Part WB and PartDesign WB can be done, but it requires a careful process. It appears your attempt at fusion mixes bodies and pads inside of bodies. That is not supported and will not work.

Do you have the Dependency Graph installed? If so, it shows several errors related to incorrectly linking Part and PartDesign WBs.

If you do not have the Dependency Graph, see https://www.freecadweb.org/wiki/Std_DependencyGraph

If this is indeed a single solid object I would try to do the entire design in a single body in PartDesign. Just keep adding and subtracting with sketches, pads, and pockets. You will probably find adding a datum plane or two useful as well.

If you have not done any of the FreeCAD tutorials, specifically featuring PartDesign, I highly recommend that you give it a try.

https://www.freecadweb.org/wiki/PartDesign_Workbench gives a summary of the current state of the PartDesign WB, and has several useful links.

Finally, forget almost anything you learned years ago. FreeCAD is not SolidWorks. It has many of the same capabilities, but the process is different. If you want to be successful with FreeCAD you need to learn the FreeCAD methods, whether you consider them right or wrong.

Gene

[chrisb]

Finally I had a look at your file. First thing I see in the dependency graph is that Body002, Body003, Body004, Body005, Body006 are empty. You can delete them without loss.

I would second Gene's suggestion to model this completely in PartDesign or if you prefer completely in Part workbench. In PartDesign you almost never really need boolean operations. The idea behind a feature is creating an object and applying a boolean operation at the same time, all additive features are fusions, all subtractives are cuts e.g. to pad=extrude+fusion, pocket=extrude+cut, ...

[chrisb]

Here is a rework with the following remarks:
- There is no need to fully model MotorBracketHead and then remove half of it.
- There is no need to add this complicated construction geometry to sketches ScrewBaseSketch and ScrewSpaceSketch. You can enter the distance as expression 35.1/2
- No need to model the holes in the hex srew, you remove them anyway.
- Note that I reversed the attachment of ScrewSpaceSketch, in order to use Length1 and Length2 in the same way as for the corresponding pad.
- I used external geometry to place both sketches in the same place

The final model contains 1 Body, 4 features and one mirror, the latter using 3 features.
The old model contained 8 bodies, 2 Mirrors, 4 Booleans, 5 Features, several of them reused in Part Booleans.

I don't know SolidWorks, but it can't be that complicated. So Gene is probably right, that it leads you on the wrong track. Be open minded, work through some of the tutorials, and learn FreeCAD from scratch. With your background, you will learn fast.

[usertogo]

- There is no need to fully model MotorBracketHead and then remove half of it.

I made a fresh start even though I have still gone that lazy route to design half (if not even 1/6th) of the design where i then was again able to complete the whole body mirror (in the Parts Workbench) but again Part Design wont have any of it and I need a whole body circular pattern which the
Anyhow the latest is again here:

delta28BYJ-center02.fcstd
in https://www.thingiverse.com/thing:3368982

If you can find a way to polar pattern the entire body around those 120deg Faces with center hole (3x polar pattern) I' be interested to know about it...

By the way that https://www.freecadweb.org/wiki/Std_DependencyGraph Utility is golden! I would wish for the programmers expanding further into the visualization tools, but hopefully with modify (program) either place with full back and forth integration...

[chrisb]

If you want to polarPattern a whole body, use Draft Array on it.

[usertogo]

If you want to polarPattern a whole body, use Draft Array on it.

Looks possible, _except_ I cant edit the 3d coordinates that would define the center of the circular (polar) array...
This tool is apparently pre 'GUI' and unless I find out how to modify the relevant data fields, or translate the whole object so that the default axis is the objects real rotational center, it did not solve my requirements...
i am able to modify simple data fields, only for 3d vectors there must be a trick I am overlooking...

By the way the issue that I am no longer able to view or edit consumed sketches or even rename those design elements must be an issue that deserves some attention. There must be a mayor problem if the design history is ever corrupted or lost?

[chrisb]

By the way the issue that I am no longer able to view or edit consumed sketches or even rename those design elements must be an issue that deserves some attention.

Where does this occur? I can always edit all sketches.

[Roy_043]

By the way the issue that I am no longer able to view or edit consumed sketches or even rename those design elements must be an issue that deserves some attention.

Where does this occur? I can always edit all sketches.

I have seen sketches that are invisible when you try to edit them. This seems to be caused by parent objects that are invisible as well. For an example see the attachment here.

Code: Select all

OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15697 (Git)
Build type: Release
Branch: master
Hash: dedaa807629ab25cf32977d30bf7610f1346aff7
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: Dutch/Netherlands (nl_NL)

[chrisb]

This seems to be caused by parent objects that are invisible as well.

That's right, if a body is hidden the sketches inside are hidden as well, even in edit mode, which I feel as well is a bit cumbersome.

[usertogo]

Sorry for not verifying that (sketches tha became inaccesible) they are in here: https://www.thingiverse.com/thing:3368982
The sketches that become invisible I learned to turn on via the property field. But I commented previously that make visible to show/reuse may have to be further graduated by configuring to also show aux and implied (centermark of a circle) geometry. Example: Very likely you would some day require a datum plane defined by an aux line and a center...

I was looking at https://www.freecadweb.org/wiki/Std_DependencyGraph to deduct and it seemed that it happened when the main Box was left by doing something in another workbench...

Right now I am going to start over again on delta28BYJ-triMount03.fcstd (Thingiverse link) because fixing/modding the first sketch - totally messes the rest up...

So here are some more observations on that process backed up from the gitter chat:

Suggestion: Sketch Solver in PartDesign Workbench: Why not instead of going into shock on 'redundant Constraint' (with blocking normal operation and obligatory click here to highlight them) just add a statusFlag (redundant/conflicting/ok) in the constraint list that is always shown. Also I am not sure if there are setting that I could modify to improve the findability of which constraint is which in the actual sketch... I suppose highlighting/coloring redundant or conflicting constraints in the sketch would also be very desirable...
Oh in the sketch The color of everything changes to green when all is 100% defined, is that not possible to do earlier to make it easier to create color distinction for any still floating geometry?

extra Bonus: sketch relation midPoint/goldenRatioPoint would be really cool some day (low priority though)
aditional Bonus: mirror sketch elements: draw half plus construction line select and be done... (low priority ...)

bonusPriority: if trim relation is applied to a line - first remove any 'equal length' relation it may have...

-Big (probably known) problem report on changing early sketches - how to prevent that that totally messes up later following features? There must be a lack of maintained relations that even get the plane 'forgotten' (switched to unrelated other face probably) - needless to say there will be probably no valuable recompute and the body just doesn't update

PartDesign Workbench suggestion: is a 'rollback bar (as known from Solidworks for example) realisticly thinkable in FreeCAD - or is FreeCAD effectivly no history based parametric modeler? That reminds me that If you were able to cleanly distinguish relations (lets say of a sketch plane) to a line or face of a prior design element, then even enabling or disabling any features in the design history should become realistic, no?

To all developers - would that be a pull request if somebody wanted to learn how to add an added option package along the lines of 'Apply feature at offset from sketch plane' ? While they are at it - a question is that data element that provides the answer to the question of the of the measure of from where to where a feature (pad/pocket etc) is applied based on objects to could learn to have a 'offset (even if resolved relative to an Offset from any other reference object (pointsource) that provides a reference of any object parallel to the normal sketch plane?
other subject: Is it supposed to be normal that you can not rotate the 3d object while in any sketch, or does that depend on the Gesture mode?

completely different subject - who would like join forces to initiate a crowdfunding campaign to invest in FreeCAD development?