Creating a thread: Unexpected results

[jmaustpc]

I used boolean union, but it only succeeded unioning one cylinder with one thread.
The other thread I'm unable to union.
Also each union takes about 10 minutes on a fairly modern laptop (8 cores i7 cpu).

If you posted your last fcstd file perhaps we could find the fault,....

The time is partly why we do not normally model threads that are not needed, however it sounds like you have an invalid solid somewhere which may be partly why it takes so long and then the fuse fails. Check each solid, back through your model history, with Part Menu...check geometry... and see if it shows any errors...

All of this is also dependent on your specific version of OCC or OCE....which your "help about FreeCAD data" would have provided...I can guess that you are using the default OCE from ubuntu 14.04 which is OCE 0.15?

If you compile OCE with TBB enabled you can make an improvement with some limited operations on multi core CPUs because this is a multi thread lib... The speed gains are very large with 8 cores but only for very specific parts of the OCE job so over all the speed improvement made little difference in some recent testing I did....but these improvements, or lack there of, are all highly OCE version and job specific.

I have several version of OCE on my system, when I have a failure of a sweep or a Boolean etc... I often try different versions with sometimes different results.


As I said the file you posted only contains a part of your model, so I can't see the failure you are talking about above.

[arcol]

For the Help->about info, please click the link on my signature.
I collect every details there, to avoid confusion. (If someone reads back a question some months later).

I use the latest ubuntu stable ppa, since yesterday. The OCC version is 6.7.0.

Since freecad never succeeded to create a drawing from it (waited an hour or so), and I
have not saved it the step before, I had to recreate the model.
Now it succeeded the boolean operation. Took quite a time, but did it.

Two questions remain:

1) Why the thread has double top. (see my previous post, I attached a picture)

2) How can I create a drawing from it.

Here is the remade model (8MB):
rod_both_end_threaded.fcstd

[jmaustpc]

2) How can I create a drawing from it.

I think there might be a bug here...I'll be back in a bit

[ulrich1a]

Two questions remain:

1) Why the thread has double top. (see my previous post, I attached a picture)

There is an extra line created, which comes from the seam point of the circle. You have a similar line along the cylinder part of your model. And you can see by inspection of your model, that the middle line in the outer part of the thread starts at the seam line of the cylinder. You may avoid this line by rotating the first face, which has to be cut with the screw profile by 180° before the cut. You will get a better looking version of your model, if you set the "maximal deviation ... " to 0.1 or 0.05% in the preferences / Part Design / Shape View.

2) How can I create a drawing from it.

I succeded making a drawing from your model in the drawing workbench. I first made a Drawing by selecting the A3-template.
Then I selected the "Fusion" and clicked "Insert a orthografic projection ...". It took minutes to generate something but it succeded.

I nearly never got a perfect drawing from a thread so far. Some lines were always missing. May other methods gives better results in a drawing. But I did not test all methods in a drawing, so I can not give a definite answer at the moment. It may also depend on the version of OCC, which was in this case a very old version.

Ulrich

OS: Debian GNU/Linux 7.5 (wheezy)
Word size: 64-bit
Version: 0.14.3692 (Git)
Branch: master
Hash: 1124a5751456ac6b8f9d6f1b470281ca67e572e2
Python version: 2.7.3
Qt version: 4.8.2
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.5.2

[NormandC]

Thread are never, ever displayed realistically in technical drawings. It is insanely computer intensive for no good purpose. There are ways to represent a thread on a 2D drawing. Machinists know to interpret these schematic representations.

http://www.en.technisches-zeichnen.net/ ... hreads.php

The major diameter will be dimensioned, and a leader will inform of the thread denomination (for example: M6 x 1.0). Also the length of the thread.

This was developed back when 3D CAD or even computers didn't exist but still remains true. In all 3D CAD software threads are commonly only represented as texture, the model also contains the thread info so when you create a 2D view of this model, the proper way of representing the thread is automatically added to the view.

[arcol]

Thread are never, ever displayed realistically in technical drawings. It is insanely computer intensive for no good purpose.

I have some part, which I want to be 3D correct (ie. print it).

And I have some other part which I want to model it, but I want to give to a "machinist".

In the latter case, I have no idea, how to generate technically correct drawings from a 3D model.
Can you help me? Maybe I should start a new thread for the drawings problem.

[NormandC]

In the latter case, I have no idea, how to generate technically correct drawings from a 3D model.

Unfortunately, I don't see how it can be done from a 3D model in FreeCAD at this point. It might be simpler to make a 2D drawing for the machinist rather than a 3D model. It could probably be done in FreeCAD, or it could certainly be done in LibreCAD.

Can you help me? Maybe I should start a new thread for the drawings problem.

Sure! Yeah a new topic may be best.

[teus]

Here is a guide how to make a thread with the gui. It makes a thread with the z-axis as the thread-axis. The Thread_cut_profile makes a standard screw profile according to ISO.
1. make a cut profile as given in the attachment. Edit the sketch and set the pitch and the nominal diameter according to your needs. Filter the constraints to named, in order to see those constraints.
2. make a helix1 with height identical to the pitch and the pitch identical to the thread pitch and a helix radius of 0.42*nominal diameter of the thread.
3. Sweep the cut profile along the helix1. Set make solid and frenet to true.
4. Make a circle with nominal radius of the thread in the x-y-plane.
5. Make a face from the circle. (Part-workbench: advanced utility to create shapes)
6. cut the face with the sweep profile
7. make a clone from the cut (Draft workbench)
8. Downgrade the clone in order to get a wire. (Draft workbench)
9. Make a helix with radius of nominal radius of the thread and a pitch of the thread and the height of the needed thread.
10. Sweep the wire along the helix. Set solid and frenet to true.
You are done. The thread may not look good, so the tesselation parameter in the Preferences, Part design, Shape view may be set to 0.1%. The thread I made with this guide was valid in the geometry check.

Ulrich

this is impossible for an amateur to follow.
I've followed the video on https://www.youtube.com/watch?v=fxKxSOGbDYs , I can follow the steps but in the end I only get one twist on the thread. Too complicated, too many steps. Making one twist of thread is easy, cloning it is incredibly cumbersome.
There's a macro for making thread, but only metric I believe, and I need square thread

[Kunda1]

this is impossible for an amateur to follow.

OP you realize your posting on a 5 year old thread? Please open a new thread and reference this one.