Strange boolean operation

[angow]

After I try a second boolean operation something goes wrong. The first cut always disappears and the second cut looks same as the first one.

If I export to step there is only one cut visible in Inventor depending on which cut I had selected before. If selected both there is only the second one visible.

I am on Vista using FreeCad 12 v5284
The onboard graphic on my notebook isn't the best and 4 years old but at least the export should work.

Do I anything wrong?

Fred

[ccccrnr]

same thing happens for me, but i didn't try to open in AutoDesk Inventor but i'm on 49xx version of freecad, so i lag the best features

[NormandC]

Hi Carlton,

The Ubuntu PPA doesn't have the same numbering as the Windows packages or the svn, because it's the Bazaar's numbering, not svn's. Your bzr4972 package is the same as svn5332. So your package is actually more up to date than angow's.

From what I can understand, these numbers won't matter soon when the developers switch completely to Git system, since it uses hashes instead of numbers for commits.

[NormandC]

Hi angow,

Do I anything wrong?

Yes, you are mixing up your history tree. (cccrnr made the same mistake if I remember correctly)

Always work on your latest object in the tree. It is the only one that should stay visible. Each time you make a new operation, a new solid is created, and the previous one is hidden automatically. You must leave it that way, because this shows you the history of your object.

If you go back on a previous object/operation and make operations on it, then your last one will not be updated. You're in effect forking your object in two separate "timelines". If you're a sci-fi fan you'll understand that: don't do time travel, it always f*** things up!

[NormandC]

BTW why are you doing boolean operations here? This should not be necessary.

Your model has only pads, which add material. When doing a hole, use a pocket feature, it removes material instead of adding it.

Edit: I added a quick (and it is this time ) video about the object's history : Project history

But I may have been too short this time...

Upcoming video: working with pads and pockets.

[NormandC]

2nd video: Pad & pocket workflow

I reuse your file and existing sketches and show how to replace the boolean operations with pocket features from the Part Design workbench. This also creates a "cleaner" history tree.

[angow]

BTW why are you doing boolean operations here? This should not be necessary.

I did what I have always done for years using AutoCad, MDT for NURBS ( without parametric) and 3D Max.
I never have been so confused as with FreeCad. This is due to the parametric system and exceptionally this heavy history-tree-feller-working- workflow
It is not so easy to get used to it if you are spoiled from the other programs.

Anyway, thanks to your helpful video tutorial...
(great as usual - and don‘t fail to publish!)
...I came a bit further



Now there are new questions coming up.
I noticed that it seems to be impossible to create more than one pocket on a sketch.
Do I have to make a sketch for each pocket even when they are identical?
What do I do if I have a lot of equal pockets?
Is it possible to constrain them anyhow?

In my next example I would like to “copy” the mount to the opposite position.
Is there a way to do anything like that?

Fred

[kwahooo]

I did what I have always done for years using AutoCad, MDT for NURBS ( without parametric) and 3D Max.
I never have been so confused as with FreeCad. This is due to the parametric system and exceptionally this heavy history-tree-feller-working- workflow
It is not so easy to get used to it if you are spoiled from the other programs.

It's easy to get if you are spoiled by Pro/E or Solid Edge, but if you used to use ancient AutoCAD workflow, it isn't:D

(great as usual - and don‘t fail to publish!)

Btw Normand doesn't like Youtube/Vimeo and other videos-sites;)

Now there are new questions coming up.
I noticed that it seems to be impossible to create more than one pocket on a sketch.
Do I have to make a sketch for each pocket even when they are identical?
What do I do if I have a lot of equal pockets?
Is it possible to constrain them anyhow?

In my next example I would like to “copy” the mount to the opposite position.
Is there a way to do anything like that?

If you need eg. two holes on a single face, simply sketch ones in a single sketch. But you cannot use one sketch to two pockets on different faces now. Jurgen is working on a Pattern feature, so you have to wait...

[NormandC]

Hi angow,

I keep forgetting about AutoCAD. I started using parametric modelling in 1999 when I learned Mechanical Desktop. I had a short course on 3D modelling in AutoCAD, but disliked it. I thought it was stupid to make you create a cylinder intersecting your model and then do a boolean cut just to make a silly hole.

I now understand that parametric modellers offer such functions as holes, but underneath the process is exactly the same, it's just hidden to the user.

By the way, I see in your model two boolean cuts where you could have used pockets.

Right now, you have two separate solids: the base plate (Cut) and the Pocket001 feature that you're going to fuse together sooner or later. If you had used only pockets, you would not have to use boolean operations.

But! Here it might prove the right thing to do, because of limitations in the Part Design workbench.

I noticed that it seems to be impossible to create more than one pocket on a sketch.

Well the rule is one sketch for one feature. I don't think it's allowed or good practice to reuse the same sketch for different features. But:

• Your sketch can have more than one element. In Sketch003, you could draw both hexagons. More generally, you can have more than one closed profile in a sketch. It used to create problems earlier in development, but now it works pretty well.
• You can copy-paste a Sketch. Then, modify the copy. For example, copy-paste Sketch003, and in the copy, move the hexagon to the other side.

What do I do if I have a lot of equal pockets?

For now, you have to work as I said above... But patterns of features (rectangular or radial) are planned for v0.13.

Is it possible to constrain them anyhow?

Not at this time. A pattern of features won't need constraints, it will allow to change the initial parameters (how many rows/columns, ...)

In my next example I would like to “copy” the mount to the opposite position.
Is there a way to do anything like that?

Not with Part Design at the moment. But you can, with the Part workbench. For that, use the Mirror command. Here, select YZ as the mirror plane, and set a base point along the x axis so your mirrored copy is at the right distance.

[NormandC]

(great as usual - and don‘t fail to publish!)

Btw Normand doesn't like Youtube/Vimeo and other videos-sites;)

It's mostly that I hate Flash and closed, proprietary formats. But since YouTube was bought by Google it offers its videos in open-source WebM format. Still, as kwahoo noted in the past, it's a pain on Linux, because we create .ogv video and have to convert it to another format anyway or YouTube will garble the video.

And I found out that Openshot can't read an ogv video with sound correctly. The video timeline is all "shot to hell". So I need a good Openshot alternative to convert my ogv videos to something else...