FreeCAD Challenge 2019-06 June - Hole Punch

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Boneshaker
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Location: Emden, Germany

FreeCAD Challenge 2019-06 June - Hole Punch

Postby Boneshaker » Sun May 26, 2019 8:48 pm

Topic for general discussion / rules / proposals:
https://forum.freecadweb.org/viewtopic.php?f=24&t=36615

Source:
https://ulrich-rapp.de/stoff/pc/cad/index.htm

You need following files:
https://ulrich-rapp.de/stoff/pc/cad/Locher/Locher.pdf
https://ulrich-rapp.de/stoff/pc/cad/Loc ... platte.pdf
https://ulrich-rapp.de/stoff/pc/cad/Loc ... platte.pdf
https://ulrich-rapp.de/stoff/pc/cad/Loc ... nteile.pdf
https://ulrich-rapp.de/stoff/pc/cad/Loc ... platte.pdf
https://ulrich-rapp.de/stoff/pc/cad/Loc ... nteile.pdf
https://ulrich-rapp.de/stoff/pc/cad/Locher/Boden-BG.pdf

This design is made by a german teacher. In his imprint he states that all his files are published under CC BY-NC-SA 2.0 licence. So please respect his rights.
https://creativecommons.org/licenses/by-nc-sa/2.0/

Translation for the parts

Pos. 01 - 17 Gesamtzeichnung des Lochers - hole punch assembly / overview
Pos. 01 Grundplatte - base plate
Pos. 02 Oberplatte - top plate
Pos. 03 Säule - pillar
Pos. 04 Hebelachse - lever axle
Pos. 05 Hebel - lever arm
Pos. 06 Druckstift - pressure pin
Pos. 07 Lochstempel - punch
Pos. 08 Lochplatte - hole plate
Pos. 09 Magnetplatte - magnet plate
Pos. 10 Bodenplatte - lower cover
Pos. 11 Anschlagschieber - paper guide
Pos. 12 Anschlagführung - paper guide bearing
Pos. 13 Magnet - magnet
Pos. 14 ISO 4762 - M4x12 Innensechskantschraube - hex socket screw
Pos. 15 ISO 2338 4 h8 x 14 Zylinderstift - cylinder pin
Pos. 16 ISO 4027 M4x5 Innensechskant-Gewindestift - hex socket set screw
Pos. 17 Feder - spring

Fase - chamfer
unbemaßte - undimensioned
geklebt - glued
nach Montage bohren - drill after mounting
scharfkantig - sharp-edged
Innenkontur der Grundplatte - inner contour of base plate
Mitte des Lochers - center of hole punch
Bemaßung unvollständig - dimension incomplete
Attachments
Hole punch.png
Hole punch.png (40.41 KiB) Viewed 1159 times
Last edited by Boneshaker on Tue May 28, 2019 3:09 pm, edited 2 times in total.
kisolre
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Joined: Wed Nov 21, 2018 1:13 pm

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby kisolre » Mon May 27, 2019 6:52 am

unbemaßte - undimensioned - for the paper pieces volume radius.
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Boneshaker
Posts: 69
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Location: Emden, Germany

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby Boneshaker » Mon May 27, 2019 11:32 am

kisolre wrote:
Mon May 27, 2019 6:52 am
unbemaßte - undimensioned - for the paper pieces volume radius.
thanks, edited the first post

If there is something unclear about the drawings nobody should hesitate to ask.
kisolre
Posts: 748
Joined: Wed Nov 21, 2018 1:13 pm

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby kisolre » Mon May 27, 2019 6:27 pm

Here is my result. All bodies modeled around respective drawings 0,0. I tried to use different techniques where applicable.
For the drill holes I used the PartDesign Hole feature. But since the depth in it is to the tip of the drill I used some sketches to find the depth based on cylindrical depth as dimensioned in the drawings.
For Lower cover I used PD Thickness and PD Draft.
I used Fasteners WB for the screws but had to model a simple set screw because could not find it there.
Pins are modeled after ISO 2338 found online (TME.eu).
For the springs I used hexagonal cross section and 5 turns (design requires 8) for ease of calculation and smaller file size.
Also made some simple sketch kinematic so when the lever arm(the LeverArmAssy) is rotated punches are driven down and springs are compressed.
2019.06_HolePunch_kisolre.JPG
2019.06_HolePunch_kisolre.JPG (155.75 KiB) Viewed 953 times

Code: Select all

OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.16687 (Git)
Build type: Release
Branch: master
Hash: ff1fb11af15a7c5f7f0ba3ef79588e128f397c2c
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Bulgarian/Bulgaria (bg_BG)
Attachments
2019.06_Hole Punch_kisolre.FCStd
(966.74 KiB) Downloaded 32 times
Last edited by kisolre on Tue May 28, 2019 2:43 pm, edited 1 time in total.
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Boneshaker
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Location: Emden, Germany

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby Boneshaker » Mon May 27, 2019 9:38 pm

Well done and very fast.
For the drill holes I just added 1 mm, don't wanted calculating. For me it is not practical to give a dimension on the edge of a drill, cause on a drill press I would measure the depth from it's tip.
Will post my fcstd file tomorrow.
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ppemawm
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Location: Manhattan New York

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby ppemawm » Tue May 28, 2019 12:34 pm

Thank you for posting your model.
There is much to be learned by reviewing others' techniques, both for beginners as well as experienced users.

I have a some questions/comments:
1. Why did you choose to offset the model from the global origin?
2. Please note that p1chamfer fails at 1 mm (V18.16093+17 Win)
3. You used Body placement to locate each component. Did you do this before or after creating the body, i.e. did you create in context?
4. Why did you not attach the spring cross-section sketch normal to the helix shapebinder?
5. If you want to save some time, set screw solid models can be downloaded from McMaster.com website, complete with threads and all details.
kisolre wrote:
Mon May 27, 2019 6:27 pm
Also made some simple sketch kinematic so when the lever arm(the LeverArmAssy) is rotated punches are driven down and springs are compressed.
Very cleaver!
"It is a poor workman who blames his tools..." ;)
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Boneshaker
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Joined: Sat Feb 20, 2016 2:20 pm
Location: Emden, Germany

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby Boneshaker » Tue May 28, 2019 2:15 pm

Hello to all,
here is my FreeCAD model of this well made design.

First I modelled the base plate, second the lower cover. So I made all empty PartDesign Bodys and Part Containers to have the whole structure. Later I recognised a Part WB cylinder isn't allowed in PD Body. Next Time I make the structure with Std Part Containers to have the ability to use Part WB.
All first sketches are symmetric to global origin or x/y axis.
Screws were made with Fasteners WB in a separate document and then copied as simple copy to save some KB. The labels I also created in a separate document with draft text string and converted to a sketch.
To align the parts I used draft/move and draft/rotate.
Added extra chamfers and fillets to pillars, punches and lever arm.

OS: Windows 10 (10.0)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.16824 (Git)
Build type: Release
Branch: master
Hash: 81ae5688d48fe9037f431b5cb8e1c9cee07f22b9
Python version: 3.6.8
Qt version: 5.12.1
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: German/Germany (de_DE)
hole punch boneshaker.PNG
hole punch boneshaker.PNG (187.8 KiB) Viewed 779 times
In the original design I discovered a minor error with the paper guide. Shouldn't be a problem in real live, but is corrected in my model.
paper guide2.png
paper guide2.png (67.51 KiB) Viewed 787 times
paper guide.PNG
paper guide.PNG (51.94 KiB) Viewed 787 times
Attachments
2019.06 Hole punch - boneshaker.FCStd
(886.83 KiB) Downloaded 17 times
kisolre
Posts: 748
Joined: Wed Nov 21, 2018 1:13 pm

Re: Freecad Challenge 2019-06 June - Hole Punch

Postby kisolre » Tue May 28, 2019 2:41 pm

ppemawm wrote:
Tue May 28, 2019 12:34 pm
I have a some questions/comments:
1. Not sure what are you seeng. Part1 is at 0,0,0. I modeled the parts so 0,0,0 will be at 0,0,0 of their respective drawings in the PDFs and dimensioned with the dimensions from the drawings so no recalculations (almost) and no wandering what is what when comparing models and drawings.
2. It should not. Did you change/recalculate the model? Could you check if there are some weird edges - double click to edit, remove ref should show all edges to chamfer which should be all bottom periphery edges:
.
Chamfer1 edges.JPG
Chamfer1 edges.JPG (109.58 KiB) Viewed 775 times
.
3. Since all parts have descriptive drawings I modeled all at 0,0,0 and then moved them inplace.
4. What would be the point? Using expresions (when they are not very complex) and named reference constraints seems the easiest and more robust way to me. Check the positionig of the set screw hole sketch (Part5/LockingHoleSk)
5. It turns out that I had that bookmarked but never used it. We should push that some setscrews are included in the Fasteners WB.

For the kinematic I would realy love to be able to attach bodies to other things. Or at least generate expressions for the placement to act as attachment :)
Last edited by kisolre on Tue May 28, 2019 2:48 pm, edited 2 times in total.
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Boneshaker
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Re: Freecad Challenge 2019-06 June - Hole Punch

Postby Boneshaker » Tue May 28, 2019 2:45 pm

ppemawm wrote:
Tue May 28, 2019 12:34 pm
There is much to be learned by reviewing others' techniques, both for beginners as well as experienced users.
Considering a look at your master piece models, reading this from you is a great honour.
ppemawm wrote:
Tue May 28, 2019 12:34 pm
2. Please note that p1chamfer fails at 1 mm (V18.16093+17 Win)
3. You used Body placement to locate each component. Did you do this before or after creating the body, i.e. did you create in context?
5. If you want to save some time, set screw solid models can be downloaded from McMaster.com website, complete with threads and all details.
2. Doesn't fail for me with 0.18.16110, chamfer works up to 2,1 mm.
3. I gave each body it's placement after creating it. Did an error with the cut outs for the paper guide, which I corrected in place. Also the chamfers and fillets I add after placement.
5. Thanks for the hint. Unfortunately threads result in a large file size.
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ppemawm
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Location: Manhattan New York

Re: FreeCAD Challenge 2019-06 June - Hole Punch

Postby ppemawm » Tue May 28, 2019 5:25 pm

Thanks for your comments.
kisolre wrote:
Tue May 28, 2019 2:41 pm
1. Not sure what are you seeng. Part1 is at 0,0,0. I modeled the parts so 0,0,0 will be at 0,0,0 of their respective drawings
Ok, I understand why now. I almost always try to locate planes of symmetry of the assembly at the global origin irrespective of the drawings. It seems easier to mirror bodies. And, I prefer to locate each body first before starting the model so as to design in context of the assembly.
kisolre wrote:
Tue May 28, 2019 2:41 pm
Did you change/recalculate the model?
I downloaded your model again and the p1chamfer seems to be working just fine. I must have corrupted the file somehow when reviewing it.
kisolre wrote:
Tue May 28, 2019 2:41 pm
4. What would be the point?
The sketch should be normal to the helix sweep path in order to have a true spring shape, especially for large pitches.
"It is a poor workman who blames his tools..." ;)