Cut Holes in Solid?

[runsva2001]

I have the following 4 sketch circles on my solid:

I wish to carve out through holes along these 4 circles out of my solid.

Attempting to use the "Extrude" tool, as I usually do when making holes out of sketch circles, doesn't allow me to create holes as it usually does. Instead it creates additional cylinders:

Attempting to use the "Hole" tool results in the following message:

Attempting to use the "Trim" tool results in my entire model being deleted:

My initial thoughts for the cause of these errors might be because the drawn sketch circles cover several different surfaces.

I wanted to try and combine all the surfaces that the sketch circles cover into a single surface, however now the "Stitch" tool for some reason doesn't let me select the individual surfaces that the sketch circles were drawn on. It only lets me select the entire solid at once:

What is going on here? Why am I now not able to create these 4 simple holes in this model?

I attached the model file to this post.

Thanks for reading my post, any guidance is appreciated.

[kacper.suchomski]

Hi

Your file is a surface corpus; has no solids.
View model status in the browser. Lots of surface bodies, no solid bodies.

Delete face 1 converted model from solid to surface body.

Repair model history.

[runsva2001]

Thanks for your reply;

I'm sorry, but I don't really understand what you are reccomending me to do.

If I open the "Surface Bodies" section of the model explorer, I see the following list:

According to this list, there are many surfaces and a single solid in my model.

Hovering my cursor over the single solid present in the list above, reveals that solid comprises all of the model. Therefore, my model here should be a solid.

If my model indeed is not a solid, how do I go about combining all the surfaces into a single solid?

Attempting to use the "Stitch" tool doesn't allow me to select individual surfaces, only the entire model at once, and attempting to use the "Combine" tool results in an error message stating that there are less than 2 solid bodies.

[kacper.suchomski · Accepted solution]

There is no solid there. Simply one of the surfaces is called a solid.

Edit Delete Face operations. They turned the solid into a surface, as I mentioned in the first comment.

[runsva2001]

Thanks for sharing this video, it cleared up some confusion to what is going on.

However, I'm a bit confused as to why deleteing those faces resulted in the solid being turned into a surface. Doesn't the "Stitch" command bring those surfaces back into a solid?

I can't simply revert all the Delete Face commands here, because I would lose a lot of progress. How do I combine the surfaces into a solid?

[kacper.suchomski]

You won't lose anything except the last Sketch. The other operations are like fighting windmills, because you only fix what you broke with Delete Face.
Take 10 minutes, remove these features and fix the model.

[runsva2001]

Ok, well in that case, how would I go about shortening the following two rectangular pillars without turning my object into a surface?

If I use "Delete Face" it will be turned into a surface, and I can't just simply move the two faces upwards.

[kacper.suchomski]

Extrude, Thicken; There are many ways.

[runsva2001]

"Thicken" appears to have worked fine there.

How about making the following:

How do I go about creating a flat filling between the two pillars and the semicircle, without using "Delete Face"?

[kacper.suchomski]

Extrude

[SBix26 · Accepted solution]

I strongly recommend that you get some Inventor training.  You are making way too much work out of relatively simple tasks.

In the case you are describing, the way to shorten the two pillars is simply to edit the Extrusion features that created them and change the distance.  That's why Inventor and similar applications are referred to as parametric modelers-- they keep track of the parameters used to construct the model, and the parameters can be altered, thereby altering the model.

Those two pillars were formed by Extrusion5 and Extrusion6 with separate but equal distance parameters (why didn't you pick both profiles and extrude them as one operation?), so you will have to edit each one separately.  This would be a good time to make them the same parameter, by the way-- d118 is one of them, and d120 is the other, so make d120 = d118 instead of d120 = 30mm.

I've looked ahead in your model browser and found the the circle feature depends on the end of one of the pillars, so that will get messed up when you change the length, but that's fixable.  Every prior sketch and feature can be edited, so there is no need to keep hacking away with Delete Face and extrusion cut features.

Post what you're trying to achieve, and several folks here will jump at the chance to show you more efficient ways to model it.  And get some formal training, either with a local VAR or by tutorials on line.

---

Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2