Help Getting Started modeling parts

[wmayer]

As j-dowsett said, Export menu is greyed out when there is no object selected (be it a Page or a solid model), but it's odd that Save and Save as were greyed out too.

If the drawing view is the active view then Save and Save As are greyed out, too.

[ccccrnr]

Wire frame is available under 'Display Modes' on the 'View' properties of the part in question (the lower portion of the side tab).

May I make a suggestion to improve FreeCAD? Could the redundant vocabulary be changed/removed?

FreeCAD --> View --> Display Mode --> has the options Docked, Undocked, Full Screen
and this is also available by Right click part
OR
FreeCAD --> Left click part --> Project --> View --> Display Mode --> has Flat Lines, Shaded, Wireframe, Points
a little bit of confusion in english


Thank you for helping me j-dowsett, i wondered if that was a another missing feature

And i got my 3D parts and i like them


the 2 long blocks with my name were done in SolidWorks2010 and SolidWorks2011
the PE was done in FreeCAD

Print on Stratasys Dimension Elite in ABS p430
in 1/10,000 of an inch layers

the FreeCAD block didn't match exactly to the SolidWorks blocks because ofthe way features are constrained. Where in FreeCAD everything is referenced to the Datam Axis, and SolidWorks let you place constrains on any feature relative to any other feature. And SolidWorks has a 'tape measure tool' to double check things and FreeCAD doesn't yet.

but overall i'm pretty happy

[wmayer]

May I make a suggestion to improve FreeCAD? Could the redundant vocabulary be changed/removed?

FreeCAD --> View --> Display Mode --> has the options Docked, Undocked, Full Screen
and this is also available by Right click part
OR
FreeCAD --> Left click part --> Project --> View --> Display Mode --> has Flat Lines, Shaded, Wireframe, Points
a little bit of confusion in english

What do you suggest? Maybe "View mode"?

[yorik]

"FreeCAD->Views->Document windows" maybe?

[NormandC]

Hey Carlton,

Those printed parts look very nice! At work we've been ordering printed parts from a supplier with a Dimension Elite machine, it's cool because we can try things out before spending the big bucks on injection molding (we work with steel mostly, but order some custom plastic parts). But I've been bugging my boss to build a RepRap (see this topic) since it would be cheaper in the long run, we could afford to print a lot more prototype parts, plus I'd get access to the machine to print personal projects!

Tonight I went back on your Index Arm part, and was finally able to get a working workflow for the fillets to succeed. I don't know if the fillet between the cylinder and the block is supposed to go all around?



Here's the file so you can study how I did it. Some pointers:

• The Open CASCADE kernel (or FreeCAD?) is very flaky with fillets. Two fillets must not meet or the feature will fail (by either disappearing, or loosing faces). There was such a problem with the 1mm fillet around the top 16Ø x 3mm thick disk and the 2mm fillet on the border of the block. Reducing the outer fillet to 1,99 solved the problem.
• I couldn't get the 1,99mm radius on the border of the block to work if it met the big cylinder. The whole cylinder's outer face would disappear. So I used this workaround:
  • Model the block with the rounded end, add the 1,99mm fillet along the top edges
  • Model the cylinder separately by creating a new sketch offset from XZ plane then padding it. This create a second pad object independent of the first one.
  • Fuse the cylinder and the rounded block together with the boolean union tool from the Part workbench.
  • Any other feature (holes, the rail cutout at the bottom) can be done before or after the fuse operation.
• For the fillet on the joint line between the cylinder and the block, either select all edges, or only the one on the back face of the block, and the fillet will be continued along the joint line automatically. But only the edge on the back face will work.
• Use the Part Design fillet tool, not the Part fillet - those two, even if they have the same icon, are totally different.
• There are many different ways to model any part. This file is my 4th try, each of the four with a different workflow.

I haven't found a way to model this part without requiring the boolean operation. Maybe in the future FreeCAD's fillet feature will get more robust. But at least, there's a workaround to make it.

[ccccrnr]

"FreeCAD->Views->Document windows" maybe?

i like that, but like this
FreeCAD --> View --> Document Windows

and

FreeCAD --> Project --> "View Properties" --> Display Mode


Normand Thanks, i'll have to explore the Part workbench .. maybe this is where for me to start

[NormandC]

I created drawing views for the Index Arm part, and added dimensions from the Draft workbench.

It's rather tedious if you have many dims to add, and there are a few glitches, still it's pretty cool, it now works pretty well for dimensions in any plane! Nice job Yorik

Basically you add Draft dimensions to your 3D object. Select the working plane first, you only have to click on a face, then add dimensions, snapping to your model's vertices. Those vertices don't need to be on the working plane. Use shift key to lock horizontally or vertically. You'll get something like this:



You'll have to play with the Dims parameters, then select all the Dims objects, and click on the Draft Drawing icon.

You'll also have to tweak the ViewDims parameters to align them to the appropriate views and set font size and dim orientation.

And you'll get this:



This is my preliminary A-size template - I need to work on the infobox.

I was planning to make a tutorial to explain this in more details. Maybe during the holiday. Only 4 work days left!

[jmaustpc]

WOW!! That looks great Norm and I assume Yorik is responsible for the code?

How long has it been since we could put dimensions into a drawing?

That's a really important feature, someone should post something under "feature announcements".

Jim

[jmaustpc]

Norm do you get these error messages in report view when you open your file?

I reported it on the forum

viewtopic.php?f=4&t=2044

I just compiled the latest svn 5322.

Jim

[NormandC]

Well putting the dims on a drawing page is thanks to Yorik's work with the Draft workbench.

It's actually been there a long time, but it was many months ago that I last tested that feature. At the time there were problems with dims that were not parallel to the XY plane. The reason was, Yorik originally designed this feature specifically for the Draft workbench, which original goal was to draw 2D orthogonal views typically on the XY plane, then export to a drawing page.

Earlier this year (last February?) he tweaked his code so that dims on different planes could be exported to a page, but at the time I tested it I had some trouble figuring it out and left the matter aside (so many things to explore in FreeCAD grabbed my attention!)

So, it's nothing new really, I just now gave it a shot again, and finally understood how to set parameters such as Linewidth Modifier, Text Modifier and Shape View Direction so the dim would show correctly on the drawing.

Since it's using a feature from a different workbench (Draft), and not a Drawing workbench feature I see this as a workaround, not sure this should be announced, but it's really useful. It would be good if we could have a radius/diameter tool too.

Since there are a few specific parameters to set, I think a tutorial in the wiki would be useful, and maybe add a link to it in the Drawing module page. A video tutorial would be nice too.

Norm do you get these error messages in report view when you open your file?

Yes, I do. Yorik made a few changes on the Draft module, maybe that's the reason for these errors? It's not preventing the file from opening and being editable.