Unable to combine bodies

[ryanRM4BD]

I am having a heck of a time getting this very organic model right.  I have been able to combine several bodies, but I am not able combine the last two.  My goal is to combine the bodies so that I can split the pieces for 3d printing and gluing. Any help would be appreciated.

[Drewpan · Accepted solution]

Hi,

I also tried to get them to combine and failed and so I checked interference and came up with this.

It seems that the problem is that the surfaces are nearly coincident but not quite. When I used the press pull

command on the Base body and basically thickened the intersecting face by 0.001, it took some time to actually

compute the result but it worked.

I have attached the file for you to look at. BTW one of your sketches is not fully defined.

Cheers

Andrew

[ryanRM4BD]

How did you figure out what the issue was?  I thought I tried everything possible.  I am trying to get better, but I cannot seem to figure out how to troubleshoot things like this.

[Drewpan]

Hi,

Practice and hanging around the forum a lot. While I am not on top of all the errors that fusion throws, sometimes

there are some key words. One of the things that one of the errors mentioned was about coincident surfaces and

that got me thinking because you need some intersection of two bodies in order to combine them. That is why I

tried checking interference - if they don't interfere then they will not combine. The thickening was more of a guess

than anything else but I thought that if the error was complaining about coincident surfaces then that was the

problem, they were coincident and not interfering or touching anywhere. Thicken one up a tiny amount and see what

happens.

Don't worry about it. Just keep doing it and when you get into trouble ask for help. If someone hasn't seen it before

they will pretty much do what I did and try various things until one works.

Cheers

Andrew

[johnsonshiue]

Hi! I took a quick look at the model. The Combine error is a bug probably due to overly complex geometry and near tangency geometry. Instead of thickening the side faces and combining the two solid bodies, it might be better to extend the main faces and create a loft surface. The resultant body may not obey the design intent 100% but the geometry should be a lot simpler and cleaner. Please take a look at the attached f3d file.

Many thanks!

[evanp4509U4JZ]

One of the things to remember when looking for problems is to turn the decimal places to maximum while inspecting. Initially I assumed the decimal places acted like a tollerance for the model and the sketches but that was not so. Sometimes surfaces will show .000" from one to another and you'll fugure it is touching. If you increase the decimal places to 8 you might find it to be .00000042" away and Fusion will refuse to join them. I frequently run into this when extruding to a surface. The profile remains at the surface and is some 6, 7, or 8 decimal places from actually planar.