It would have been best to start with an additive gear. Now you can move the gear out of the body, use Part-Extrude for 3000mm reversed and make a boolean Common. If you want to continue working on it in PartDesign, you have to create a new body with Common as BaseFeature.
The file is too big to attach.
Attachments
Bildschirmfoto 2019-04-23 um 08.36.35.png (56.67 KiB) Viewed 690 times
While this will work it is not the proper way to do it. You should not use features of a body outside of the body. This will give "Links go out of scope" warnings/errors:
LinkOutOfScope_02.JPG (85.23 KiB) Viewed 688 times
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The Common operation should be done with the body itself and not with its last feature (pollar pattern):
LinkOutOfScope_03.JPG (74.12 KiB) Viewed 688 times
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and the Part extrude should be done with the gear profile OUTSIDE the body (you can drag it from the body on to the file name to do that):
LinkOutOfScope_04.JPG (91.65 KiB) Viewed 688 times
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After you do that you should yse the Common as BaseFeature for a new body if you need to continue adding PartDesign features:
Common As BaseFeature.JPG (89.75 KiB) Viewed 688 times
Another way is to convert that gear profile to sketch, (Draft/Draft to sketch), drag that to the body, draw a circle around the gear profile and use that to pocket through all:
DraftToSketch.JPG (101.87 KiB) Viewed 683 times
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But as Chrisb mentioned better start with the PartDesign Involute gear and add features to that. You already have all your sketches so this should not be very hard to recreate.
Another way is to convert that gear profile to sketch, (Draft/Draft to sketch), drag that to the body, draw a circle around the gear profile and use that to pocket through all:
In this way, be careful not to use internal involute gear, but a negative of external involute gear, because the profiles are not the same.
To make things clear: Some references became unclear due to intermediate posts:
- meme2704 and I were both referencing the original first post.
- kisolre referenced meme2704's first post, where indeed a feature is used in a Part boolean operation.
There is another way, staying in PartDesign:
- Create the gear in a new body
- Add a boolean operation in the first body
- Set the type of the operation to Common and add the second body, which contains the gear.
I should mention that the filesize rises from 1.2MB with the Part-booleans to 2.0MB with the PartDesign-booleans.
This is how the tree will look like:
Attachments
Bildschirmfoto 2019-04-23 um 12.28.15.png (53.51 KiB) Viewed 665 times
