I need to cut a groove on a flat suface transitioning to a round surface smoothly. Thank you
I created a sketch for the path on the right plane, then added a new plane to the endpoint of my sketch. I copied your profile sketch to the new plane and added a Swept Cut along the path. The corner can stay square, or you can add a fillet before creating your path (like I did) to round the transition off.
Hi Karen, Can you post your part and what version are you using? Thanks
2012 I'm not sure how to insert the part file here...
here is the dwg
Have you tried a sweep cut?
If the middle portion is flat then create an extrude cut and then add the fillets on the outer edges.
I've been using cut revolve
Click reply to the post like normal. but before you type anything select the text in the top right corner says "Use advanced editor" then you have to move to the bottom of the text screen on the left and then you will be able to browse to your files location, select file, then update.
Something like this?
Sorry, conversation evolved while I worked that up.
I posted the prt file for clarity
I got it finally...thanks!!
In order to make it a smooth transition, you will probably need to add a fillet between the flat and curved surfaces. Then you should be able to use a swept cut to make your profile.
Karen, I think if you create a plane in the middle of your groove location, and create a path sketch with a radius that you require at the flat/round intersection, close the sketch, and then create another plane perp to your path sketch, do a cut sweep, I think you should get the result that you want. You might have to play with it,..once completed, you can pattern that to have your other groove. Hope it works out for you.
giving that a shot thanks...
UGH...still can't get it.
Try this. First delete Cut-Extrude18 so that we can add the groove at the end. Then make a plane that is parallel to Top and tangent to the outside of the boss, where we want the groove to start.
Then sketch the groove profile on that plane, just like you did in Sketch21.
Then start a sketch on the Right Plane and draw the path for the bottom of the groove.
Make sure the end of the path pierces the bottom of the profile, and radius around the sharp corners.
Then do a swept cut with those two sketches.
If you need a sharp corner in the groove, do the same as above but without the internal radius.
The dims on the flat part are different than the ones that go across the top. I'm so sorry I failed to mention that. :/
Not a problem, just changed the sweep profile for the two offsets. You can add fillets if you need.
Or if the profiles are different apart from just the depth, then here is another approach. Move the Cut-Extrude18 feature to right after the Boss-Extrude3 (I also changed the sketch plane for Sketch21 to Top Plane).
Then roll forward and edit Cut-Revolve14 and change the angles to 90 degrees (I am assuming you don't want undercutting there). This will leave an empty space under that portion.
Then start a sketch on the underside of that top semi-cylinder and convert edges of that face.
Then with that sketch Extrude down to the bottom of the horizontal groove.
I'm not sure if you need the inside edge filleted.
I think this should fix your problem.
after the first groove is inserted
use the revolve feature with the groove in the feature
remove the boss remaining
Karen, hope my attment is there...here is the groove. i did a section cut for viewing.
I can see it...I need a sharp corner...but I think I can work around it...thanks
u r welcome...you can also do it the way Patrick did.
hope you can get the model...our emails are somewhat locked down...i will send a pdf too.
I suppressed cut extrude 18 and some other sketches.
Take a look at the end features,,,plane 6 fille 1 and cut sweep2.
Also hit space bar you will see orient views or mine, side pete and end pete..
You can play with it and fix it how you want…
I got it! Amazing what a nights rest will do for ya! Thanks everyone for all your help!
Retrieving data ...