What are the right tools and sequence to use to create a so called imprint or a cavity or a nest for a part that was imported from a STEP file.
Lets say the nest has to be 1mm wider than the part that goes inside it.
And if a part needs to be fully "submerged" inside the nest I want the nest to remain open from the top.
Imagine a ball inside a deep hole. For you to be able to place the ball inside a hole, the top of the hole needs to be larger than the ball diameter.
A simple boolean operation would not do that because if the ball is more than half way in the hole, the top is closing up.
I find it very difficult because NX is new to me.
Emboss body seems to be the right tool but does not work... it fails if I increase the clearance to anything other than 0. Might be related to my specific STEP file.
I somehow need to find the external dimensions of the part and extrude it upwards.
Than use this newly created body and make all the faces of it half a millimeter wider
And then use an assembly cut or some other boolean operation to cut this newly created part from a block of material.
Basically I need to create a tool that I can use to cut the exact shape out of a block.
Attached is a movie file showing 2 options. The first one is probably the one you want to use as your shape is probably more complex than a sphere.... The second one is an option should your geometry be really simple - like a sphere. The example does not show the actual draft (wehen re reading your question) however whatever draft you need should be added in the Isoclina and Extrude function. I hope this helps creatiing your design.
Thank you. I already learned a lot but my part is more complex than a sphere and the "Isocline curve" gives in my case a curve that cannot be extruded.
Imagine a spoon or something like that. How do I make a cavity for a spoon?
I need to find the outline of the spoon.
I need to extrude the outline of the spoon upwards... from the spoon surface.
And then I can UNITE the new shape with the spoon, offset faces 1mm for it to be larger than the original spoon.
And then I can SUBTRACT this shape from the block of material where I need the cavity to be.
In addition you can look into NX Moldwizard which is a tool for complete mold design. With this comes all the tools needed to make both cores and cavities.
Here is an image of the process.
Tools keep failing on me... probably because I work on a dumb body that is imported from a STEP file and is a bad apple.
"Circular dependency detected
Did you try to modify the base body using something derived from an extracted or linked feature"
I love how the video is blurred out when I pause it :-)
But I was able to get your approach.
- Extract geometry -> Face -> Face Chain and selection filter "Tangent Faces"
- Extrude -> first selection filter drop down "No selection filter" -> third selection filter drop down "Sheet edges"
I had some success trying to extrude "Face Edges" but when I included one of the rounded/blended edges of the model I got an error:
"Selected faces will create more than one output body. This is not allowed in this feature"
I don't think I have the most difficult part in the world... should be a straight forward process to create a nice nest for this part.
Even projecting the curve of the parts outline is failing. "The input section is not valid" - No idea what that means.
Another thing I want to achieve is to remove the holes aswell so a boolean operation would not cause long rods to shoot out of the nest.
I will keep fighting this thing until I come up with good workflow. I am on my first days working with NX and I do not want to learn wrong approaches to simple problems.
I absolutely love this community and the video responses.
I was able to get some help from my collegues.
The solution was:
- Use "Delete face" to delete the holes and the rounded edges
- Extrude the top layer (Boolean "None" and selection filter "Face edges")
- Extrude the bottom layer (Boolean "None" and selection filter "Face edges") and start at -4 mm to compensate for the material thickness
- Unite the two extrusions
- Move small faces until "motion face consumed" to get rid of the small problem area that is caused by the bottom layer being smaller in some regions than the top layer.
- Extrude yourself a cube
- Subtract the previously created body from the cube.
- Offset region to move the faces of the hole outwards to create room for the part to be placed in there.
Seems to be a bit more steps than I originally thought... or there might be a more elegant solution.
Looking at your imported geometry (from the image) it looks like you have an unfortunate undercut that needs to be dealt with - hence the extra modeling steps. In the attached movie file I try to circle the area to highlight the problem areas, the "step" produced by the isocline curve that I here use bridge curve to wipe out). With a bit of DFM the part would probably be designed slightly differently. However since this geometry is imported I asssume that you might not have a saying regarding the design bit.... However if designed differently you would not need the extra features (here bridge curves). Have a look at the attached movie maybe there is something in there for you.
All this process is an easy task for Mold Wizard but if you want to do it using normal modeling commands this is my suggestion to do this:
1- import the stp part and apply the shrinkage factors using scale body. (Doing offsets is not very good way to compensate for shrinkages)
2- create your parting lines by isocline curve.
3- create your parting surfaces.
4- create a box.
5- subtract the part from the box.
6- split the box with your parting surfaces.