Hello,
I am trying to perform a CUT operation in the Part tool and I am not getting the results I am expecting.
I have 3 parts that I am cutting with a 4th. Each is created with the sketcher. If I cut the 3 parts first then union them together, I get the part I expect. If I union the 3 parts together and then cut them, I get residuals that are not correct. I don't understand why I don't get the same results.
Here are the 3 parts:
After these are "unioned" together, they are to be cut with this solid:
If I cut each part individually (with cut parts duplicated from the original) and then union the results together, this is what I get and want:
If I union them together, then cut, I get this:
I used to be able to do this just fine. I don't know what changed or why this is happening. Any help would be appreciated.
Model attached.
Thanks,
Bill
OS: Mac OS X
Word size: 64-bit
Version: 0.14.3703 (Git)
Branch: releases/FreeCAD-0-14
Hash: c6edd47334a3e6f209e493773093db2b9b4f0e40
Python version: 2.7.5
Qt version: 4.8.6
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.7.0
Cut not working as expected. Help please.
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Cut not working as expected. Help please.
- Attachments
-
- Reed Protector.FCStd
- (76.31 KiB) Downloaded 66 times
Re: Cut not working as expected. Help please.
Try rotating Inner Barrel Sketch on the Z axis by about 10*. Go into your tree view and click on Inner Barrel Sketch. Goto Edit > Placement... and first check on the "Apply incremental changes to object placement" then from the Axis pulldown, select Z and give it an angle of 10*. Now fuse the 3 parts and make your Cut.
OCE, the CAD kernel that FreeCAD uses, sometimes has problems with the seams. Rotating the sketch will move the seam of Inner Barrel out of the Cut and you might get your desired result. That is what I had to do to get it to work correctly, though my results before were not the same as yours, probably due to using a newer version of OCE.
On a side note, this entire part could of been done completely in Part Design without the need for any Rotation, Fusions or Cuts.
Mark
OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4665 (Git)
Branch: releases/FreeCAD-0-15
Hash: f376ce13106bd0e4eca184a6faff89cc499860c0
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
OCE, the CAD kernel that FreeCAD uses, sometimes has problems with the seams. Rotating the sketch will move the seam of Inner Barrel out of the Cut and you might get your desired result. That is what I had to do to get it to work correctly, though my results before were not the same as yours, probably due to using a newer version of OCE.
On a side note, this entire part could of been done completely in Part Design without the need for any Rotation, Fusions or Cuts.
Mark
OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4665 (Git)
Branch: releases/FreeCAD-0-15
Hash: f376ce13106bd0e4eca184a6faff89cc499860c0
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
This post made with 0.0% Micro$oft products - GOT LINUX?
Re: Cut not working as expected. Help please.
I suspect this to be an occt bug. But if you already know how to reorder the booleans to get to your desired result, then you are done for now. But thanks for bringing this up, as your geometry shows interesting behavior in light of issue #1971.
Re: Cut not working as expected. Help please.
Hello wdsteck,
I'm wondering why in "Inner Barrel Sketch" you separated the inner horizontal line into two segments, one being 2mm high at the bottom?
To add on what Mark wrote, this is why cutting each part individually then union them together worked: it removed the failing condition.quick61 wrote:OCE, the CAD kernel that FreeCAD uses, sometimes has problems with the seams. Rotating the sketch will move the seam of Inner Barrel out of the Cut and you might get your desired result.
I'm wondering why in "Inner Barrel Sketch" you separated the inner horizontal line into two segments, one being 2mm high at the bottom?
I'm looking at this and the only way to make the cross-cut ending with the "V" top would be to build a helper pad (or pocket) on the base. Or are you seeing something I don't?quick61 wrote:On a side note, this entire part could of been done completely in Part Design without the need for any Rotation, Fusions or Cuts.
Re: Cut not working as expected. Help please.
To get the "V" I'd just try adding two chamfers with half the width of the slot to the edges.
Regards
Ektus.
Regards
Ektus.
Re: Cut not working as expected. Help please.
Nope, not seeing anything you don't.NormandC wrote:I'm looking at this and the only way to make the cross-cut ending with the "V" top would be to build a helper pad (or pocket) on the base. Or are you seeing something I don't?
Yes, a small helper pad would be needed, but I consider that "par for the course" so to speak. Small rectangular Pad to map one of the slices into the side then use it's edge that I placed at the center axis of the cylinder as the axis reference for the polar pattern feature. Then Pocket the helper away and we're good to go.
This would be the point where I then reference this thread - viewtopic.php?f=3&t=3907 - for those unfamiliar with the use of a helper Pad and making pockets into the sides of cylinders.
Mark
This post made with 0.0% Micro$oft products - GOT LINUX?
Re: Cut not working as expected. Help please.
If I understand this part correctly, it's possible without a helper. See the attached file for the principle (sketches are vastly underconstrained and not all geometry has been recreated, but you get the idea).
Regards
Ektus.
Regards
Ektus.
- Attachments
-
- cylinder_with_slots.FCStd
- (35.36 KiB) Downloaded 57 times
Re: Cut not working as expected. Help please.
That could work, but I was thinking about something more along the lines of the attached where I used the helper Pad, (Sketch003+Pad002). It has several advantages. First is the slots and the V's can be adjusted to length and angle by editing the sketch. and the V's have a sharp bottom, no flat. Now that flat probably would be of no consequence if one were 3D printing or even machining, so either way would work just fine for most any real world application. I just personally prefer to use chamfers and fillets in their more traditional roles, such as countersunk holes and rounded/broken edges, not as a pseudo shape for a V or U cut/channel. Maybe it's just me...
Mark
OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4665 (Git)
Branch: releases/FreeCAD-0-15
Hash: f376ce13106bd0e4eca184a6faff89cc499860c0
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
Mark
OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4665 (Git)
Branch: releases/FreeCAD-0-15
Hash: f376ce13106bd0e4eca184a6faff89cc499860c0
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
This post made with 0.0% Micro$oft products - GOT LINUX?
Re: Cut not working as expected. Help please.
Hello All,
You are all much more experienced at this than I am! I want to thank you for all the insights!!
I now understand that by rotating my original design, I get the seam out of the cut and the Union then the cut now works. Thank you for that explanation.
I am just not good enough with Part Design to tackle it in that tool. I don't envision how to make it without the sketch. I will have to play with part design to see how that tools works and what I can do with it.
The extra segment in the Inner Barrel sketch at the bottom inside is left over from printing issues. This part is a protective cap for my Bagpipe Chanter (yes, along with other personal insanities, I also play the bagpipes!). It will slide over the chanter top holding the reed when not in use. The bevel will help when sliding the protector on the chanter. We are having printing problems, however, and so I got rid of the bevel until we resolve the printing issues.
That is also the reason for not having a square inside top. The top has to be sealed but sealed gradually (>45 degree angle) so the plastic being laid down by the printer has something to sit on when forming the top. In the future, I will have a hole up there with threads for a moisture control cap for the reed, but that's another story.
Thanks again for the insights. I will re-read your posts and play with your models to see how you did all these cool things.
Bill
You are all much more experienced at this than I am! I want to thank you for all the insights!!
I now understand that by rotating my original design, I get the seam out of the cut and the Union then the cut now works. Thank you for that explanation.
I am just not good enough with Part Design to tackle it in that tool. I don't envision how to make it without the sketch. I will have to play with part design to see how that tools works and what I can do with it.
The extra segment in the Inner Barrel sketch at the bottom inside is left over from printing issues. This part is a protective cap for my Bagpipe Chanter (yes, along with other personal insanities, I also play the bagpipes!). It will slide over the chanter top holding the reed when not in use. The bevel will help when sliding the protector on the chanter. We are having printing problems, however, and so I got rid of the bevel until we resolve the printing issues.
That is also the reason for not having a square inside top. The top has to be sealed but sealed gradually (>45 degree angle) so the plastic being laid down by the printer has something to sit on when forming the top. In the future, I will have a hole up there with threads for a moisture control cap for the reed, but that's another story.
Thanks again for the insights. I will re-read your posts and play with your models to see how you did all these cool things.
Bill