Project became extremly laggy and I get this error when attempting to cut the file: Error: There was a problem combining geometry together.

[1900745KYKTT]

Hi,

I was trying to design a project based on a gameboy shell, so I went online and downloaded a .step file of the shell. I then proceeded to unstich it so I could remove unwanted holes. After restitching the object, the whole file became extremely slow. Even selecting a face took 30 seconds to compute and I got the error: There was a problem combining geometry together. I tried exporting the file as a .step file and reopenning it in a new file. This removed the lag but I still couldn't cut the body when extruding. The rare times where I managed to cut the body with an extrude function, it would extrude with a slight angle up.

I am very confused and would like to find a solution to these issues

Original file with lag is attached below and named: GB v16

Exported non-laggy file is also attached below and named: Shell v1

Thanks for the time and help

[ryan.bales]

There is a handy text command 'fusion.dumpfeaturesbycomputetime' that helps find the features that are slowing down a model. in this case, 'unstitch7' takes 352 seconds to compute that feature. 

Given the extensive surface modeling work i'd consider doing that in Direct modeling then capturing design history afterword like you've done with reimporting the exported step. This is my opinion and not necessarily 'Autodesk Support or Fusion 360' opinion. 

What/where are you trying to cut?

[1900745KYKTT]

Why is it extruding diagonaly???Thanks for the help concerning the lag. However I still get an error sometime when I try to cut using extrude function and my extrusions are still diagonal any fixes to that?

[ryan.bales]

There are a number of solutions to this:

• Remove fillets, cut the face vertically and extrude
• Create a sketch on offset plane and extrude 
• Remove all other grooves and use a pattern to pattern the completed grooves features or in this case, faces. 

This does highlight the reasoning for doing fillets last, in this case they are complicating a fair amount of the design process.  

[1900745KYKTT]

Even if I use an offset plane the problem still occur. I also cannot remove the fillets because this model was downloaded from the internet and I can't go back and remove them.

[g-andresen]

Hi,

---

@1900745KYKTT  schrieb:

 However I still get an error sometime when I try to cut using extrude function and my extrusions are still diagonal any fixes to that?

---

That is why

günther

[ryan.bales]

An offset plane off that face will fail as its still flat, if you are using that face and not something square to the body you'd need a plane at angle, which will use an edge and origin orientation.

I was able to cut away the old grooves on one side and pattern some others. This might be the best way to clear out the older geometry that is problematic and recreate new geometry. 

A lot of cleanup is still needed in this model. So many faces are off in very slight angles. 

 

[1900745KYKTT]

How did you manage to do that when I try to cut the model I get the following error:

Error: There was a problem combining geometry together.
If attempting a Join/Cut/Intersect, try to ensure that the bodies have a clear overlap (problems can occur where faces and edges are nearly coincident).

[ryan.bales]

Fusion let me do it because i owned an original GameBoy just like this one. 😄

Okay i'm joking:

• Create a surface body and thicken it to create the negative for combine/cut/boundary fill
• Then extrude a large overlapping profile to clear the old geometry
• Then back extrude that face to join the body and make it solid
• Then use combine cut to clear the new groove
• Pattern the groove face and then mirror.

Here is my version showing my steps. Again the model itself has some irregularities that complicate this process. 

[1900745KYKTT]

WOW thanks I would never have found this myself and I am still confused as to why I was getting this error!!! Do you know what could have caused the previously mentioned error?

Thanks for the help btw

[ryan.bales · Accepted solution]

I'm going to generalize in my answer because i'm not a software developer. @jeff_strater can explain far better than i can.

From what i can tell, the model surfaces of the grooves are not very exact or square, attempting to make features using them, or even combine, extrude or cuts will generally result in sliver features or errors in filling the solid volume.

[1900745KYKTT]

Yeah that makes sense. Thanks a lot for the time and effort!!! It is really appreciated!!!!!

[ryan.bales]

of course! happy to help.