Trying to add a chamfer to a model

[Joel_graff]

So before I start over from scratch on this model (I know I've messed it up a good bit), I thought I'd see i anyone can tell me what I've done wrong.

I'm trying to add a chamfer to a face along the bottom of the model (one of the large faces at the bottom of the keystem). It was successful, but I can't seem to figure out how to eliminate the portion of the pad that was chamfered. Also, I get the error:

Code: Select all

Part::Chamfer / Chamfer: Links go out of the allowed scope

which sometimres prevents the chamfer from happening.

I know it's just bad model organization that's getting me, but I'd appreciate a tip or two.

aiie_smk_keystem_2.FCStd

(74.87 KiB) Downloaded 18 times

Code: Select all

OS: Ubuntu 20.04 LTS (ubuntu:GNOME/ubuntu)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.21514 (Git) AppImage
Build type: Release
Branch: master
Hash: 89ddab33f692a9bd739171689f9ab0eb58d64b35
Python version: 3.8.2
Qt version: 5.12.5
Coin version: 4.0.0
OCC version: 7.4.0
Locale: English/United States (en_US)

[Gregory son of Carl]

I think what happened here is that you accidentally selected edges from the PartDesign body for chamfering instead of from the Cut feature on top which looks to be the cause of that error message. To clean things up a bit, you can change the "Base" object Parameter for the chamfer to the Cut object.

To deselect the chamfer edges in its current state, you need to make the PartDesign body visible before activating the chamfer Task window.

[openBrain]

This is clear from the Dependency Graph.
You have a Part/Chamfer applied on the PartDesign/Pocket.
You should either :

• Apply a PartDesign/Chamfer on the Pocket (in this case the chamfer is part of the Body)
• Set the Display Mode of the Body to 'Tip' then you can apply the Part/Chamfer (in this case you'll have to update the Cut so it uses the newly created object)
• Apply the Chamfer on the existing Cut object

[Bance]

Better to remain in PD, use subtractive cone and chamfer.

[papyblaise]

Erase all inusful sketch , use Hole instate of pocket : the cone became automaticly , and chanfer

[Joel_graff]

Ok, so I got a lot more response than I expected.. and a lot faster. Replying to the comments (out of respect for the time you guys took to make them):

Erase all inusful sketch , use Hole instate of pocket : the cone became automaticly , and chanfer

I used pocket and included the cone because this is a 3D print - those are critical elements to the design, I'm afraid.

Better to remain in PD, use subtractive cone and chamfer.

I may revisit that - Getting the cone subtraction to work properly was really tricky. Clearly, I was mixing Part and PartDesign elements, which lies at the source of my problem.

This is clear from the Dependency Graph.
You have a Part/Chamfer applied on the PartDesign/Pocket.

I initally went loking for the chamfer in PD, but didn't see it, so I tried the Part chamfer. Took another look and found it. Otherwise, applying the chamfer to the cut object is obviously the quickest fix. I suspect it would be better for me to do it entirely in PartDesign.

I think what happened here is that you accidentally selected edges from the PartDesign body for chamfering instead of from the Cut feature on top which looks to be the cause of that error message. To clean things up a bit, you can change the "Base" object Parameter for the chamfer to the Cut object.

To deselect the chamfer edges in its current state, you need to make the PartDesign body visible before activating the chamfer Task window.

I took a look at this. Your solution works, but I discovered I can't pick "Cut" as base when creating that chamfer initially. I have to choose Pocket, then go back and change it to base after applying the chamfer. That said, once I did that and hid the Cut object, the model appears as it should. Clearly, mixing Part / PD elements is the source of my issue.