Hello i have a part that has been extruded up to a body and now i need to put a 6 mm wide by 6mm deep with a 6mm rad. at the bottom in the center of the surface of the part how do i draw that on the non flat surface please look at the file attached and see if anyone can help with with this. I thank you
Aaron
SolidworksParts And Features
I'm not sure what you mean but could you extrude and use the non linear face as an end condition?
Future Version.
Can you save this as a parasolid?
could you make it clearer which surface you want it on?
like this?
thank you for all the help so far Greg you have the right surface but i need the cut to go all away around in the middle of the ring on that surface.
here is a parasolid of the file
Aaron
like this?
Aaron, here's my go with it, based on what I saw of Greg's models. Since the lower surface (radius) was formed with a loft and only four guide curves, you'll want to check it for accuracy all around before using it (6mm radius). Add more guide curves if necessary.
http://www.industrialdesignhaus.com/internet/Inner-Anvil-Trim-Jeff.zip
(My first use with surfacing within v2010. So far, so good.)
Here is what I came up with.
Is this what you were talking about?
Allen & Jeff they both look awesome It would not be asking to much to explain how you did it step by step. if not I completely understand but thank you very much for everyones help with this i was totally lost.
Thank you all
Aaron
Aaron,
I began by getting the thickness of the wall and offsetting the outer face/surface hald that distance.
I then used the extend Surface comand.
I then offset the top surface by 0 (copied it in place) and used this to trim the exetnded surface.
I did a 3D sketch and converted edges from the trimmeedge of the extended surface to use as a path.
I created a parallel plane to the top plane at a line segment end point.
I sketched the 6mm wide with radius and extended this past the top of the surface to use as the profile for the cut.
You may be able to use the Roll Back feature and examine this step by step to get an idea.
Hope this helps.
regards,
Alan
Aaron, my approach was fairly simple. Generally you can see what Alan or I did in this case by rolling back the scroll bar to the first feature that's different from what you did and then rolling toward the end of the feature tree one feature at a time. So you can see the whole chronology of the part's build this way.
I created a plane above the compound surface you've got and extruded a cut 6mm deep past that face (setting in Cut feature).
I then used Delete Face to clear out the bottom face of the groove. This needs to be replaced with the radiused face you asked for. When you delete a face on a solid body, it becomes a surface body.
The next step is to create the radiused surface at the bottom of the groove. To do this, I figured a Loft would work best, so I created guide curves (6mm radius) in four sketches around the periphery of your groove to tell the Loft operation how to form the surface. This is the area you should check to make sure it's consistently near 6mm radius the rest of the way around your groove--sometimes the Loft will tweak a bit in the areas not near the guide curves. Next I created Composite Curves of the open bottom edges of the groove surfaces. Lofts like to have the same amount of members in geometry segments if possible, and even though the Composite Curve is a bit of a dinosaur, it works well for this purpose. So I opened the Loft Surface dialog, chose each Composite Curve, chose each of my four Guide Curve sketches, and everything lined up properly so I executed the loft. Piece of cake.
The last step was to return the surfaces to a solid body, which I did by using Knit to knit each surface body together. I used the "Try to form solid" option when doing this, and it succeeded.
That's it.
Aaron - Just in case you need the slot to have sides parallel to the sides of your part, I've done the slot using a solid cut offset from your surface by 6mm then filetted the bottom of the slot. Your original post mentions a 6mm rad at the base, so I now realise I've not done the slot correctly - oops! - but you get the idea. I did this because the other guys' methods have the slot sort-of perpendicular to the non-planar surface so making it an unattractive proposition for machining (if that's what you're going to do with it). That's the way of it with swept-surface cuts unless, as has been already said, you constrain the swept cut to make it do more than the 'vanilla' cut. X_T file attached.
WOW!! you guys on here are awesome you all have helped me out thank youfor your time and effort in this. yes this will be used for a cutter path for machining again thak you ALL!!!!!!!!!!
Aaron