So, I finished my project and want to print it.
Problem is, I wanted to have a 5mm thick wall, but somehow SW doesn't let me thicken it...
I need to thicken it to the inside so I could print it (it need to be hollow on the inside to cut production costs and time), what would be the best method for this?
This is a copy of your other thread Having a problem adding thickness and mirroing a project. which I've replied to.......
Please do not make duplicate threads for the same issue.
Dave.
Sorry!
For some reason the last post took days to upload, so I thoght it had not been approved.
Run the Check tool:
Select Minimum Radius of Curvature and click check:
It tells you what the minimum radius is and even tells you where it is.
In general, whatever this value turns out to be.....your thicken thickness needs to be smaller than this.
If you want to have something thicker, you need to change that area..
Nice, thats good info to have, thank you!
Althogh it says the min radius is 2mm I can't seem to thicken it anyways =(
That's a pretty big part for 3D print.
Don't think you need 5mm thick, maybe 1-2mm.
Isn't that going to become too frail?
You can't buy gauge pod at 5mm thick.
The material only need to support itself and the gauges.
What material are you printing?
Which type of 3D printing?
You should pick material that won't soften above 80C.
I see...
I'm not that educated about priting and I don't own a 3D printer, was thinking about sending it to a printing lab.
..your MOR MRO is very small.. would suggest you redo this (only half and mirror). or, create boundaries around this and make a solid.. then rely on the 3DPrinting software to apply a wall and fill/matrix the inside.
Is this because solidworks has issues dealing with 3 point solids?
"3 point solids"... sorry, I don't understand?
I suspect he means: Non-manifold geometry
Let me see if I can explain. It is entirely possible that I am way off base here....if that is the case, I am sure that some of the Guru's will be able to redirect me.
Let's say you had this shape:
And you extruded that into a surface:
As you can see, the Minimum Radius of Curvature is 0.25 in, exactly as my original sketch showed:
Now, lets try to offset it 0.5 in:
Can you see the issue starting here?
Now, this one worked (I honestly didn't expect it to...I expected it to fail), you can see that it is not a true offset:
As this distance is NOT 0.5 in:
When you start getting into more complex geometry, the ability for the software to trim it like this lessens.
I just downloaded your project, thank you for the upload!
It seems like you managed to fill it completely somehow, wow! Trully I have much to learn yet.
Mind sharing what tool was used?
I just made sure your surface edges at the middle, where it mirrors, were not overlapping..
So anyone has any ideia?
At this point this is driving me so mad I'm even willing to pay someone to teach me how to fix this.
As others have mentioned you have minimum radius problems, which I will let you fix.
I wanted to show you a method of getting the thickest part from the existing geometry.
1. Convert your surface body to a solid. Start by doing a filled surface for the bottom opening.
2. Before doing surface fills for the 3 holes, add a Plane and create a sketch of the 3 holes using Convert Entities. Then fill those holes.
3. Split the solid body and delete half.
4. Use Check to identify where there is very little radius of curvature. Delete & Patch that surface. (You should instead be editing your surface features.)
5. Mirror body to get back to original.
6. Use Check to identify the current radius of curvature (1.56 mm).
7. Use Shell on the bottom face with 1.5mm wall.
8. Use the sketch in step 2 to cut those 3 holes.
This was really helpfull, I was able to do this as the steps you've described, thank you very much!
As a new user, you have no idea how much this helped.
Thanks again!
Samovar,..... please share how you did it.
Firstly, I was first able to do it by using the shell tool from your project, Paul, but I wanted to learn how to do it properly, so I redid the whole surfacing.
Using the check tool as described by Dan I found the piece that had the problem, and somehow the loft surface was causing the problem, so I redid the spline on that until it worked, following the steps that Bill pointed out, and the project was corrected.
Although I could do it by following the steps, the project I ended up forwarding to the printing lab was yours, Paul, after I used the shell tool for 2mm, as Frederick suggested, and recutted the holes, as in your project it ended up looking a bit nicer for some reason.
When its printed I'll send you guys a picture!
As others have mentioned you have minimum radius problems, which I will let you fix.
I wanted to show you a method of getting the thickest part from the existing geometry.
1. Convert your surface body to a solid. Start by doing a filled surface for the bottom opening.
2. Before doing surface fills for the 3 holes, add a Plane and create a sketch of the 3 holes using Convert Entities. Then fill those holes.
3. Split the solid body and delete half.
4. Use Check to identify where there is very little radius of curvature. Delete & Patch that surface. (You should instead be editing your surface features.)
5. Mirror body to get back to original.
6. Use Check to identify the current radius of curvature (1.56 mm).
7. Use Shell on the bottom face with 1.5mm wall.
8. Use the sketch in step 2 to cut those 3 holes.