Import Gerber files into altium designer

Hi,
I have tried a lot to import https://www.minicircuits.com/gerber/TB-458+.zip to extract PCB file but I was not successful.I've only see some points in PCB window and in Table->layer I can't set layer names successfully. Is it possible to import this gerber files to altium designer and upload pcb files here? and could you explain how you do that?

Altium Designer can open and view gerber files, but you can't convert them back to a PCB in any way because gerber files do not contain any information about the components or footprints that were used to generate the gerber files.

Altium can do this "reversed" operation. But it's not import. It is re-export.
In CAMeditor after loading all gerbers, place all layers in the right order via tables, after that define layer-sets (which layers are drilled with one NC-drill). Then extract netlist and you will be able to export the board to PCB Editor where you'll be able to edit your pcb.
Of course, there are a lot of restrictions. First of all, as was mentioned by ArticCynda, gerber doesn't contain any info about components, so you can drag single pads, but not "component" group of them. Second, all holes will be converted as TH-pads, no vias (nc-drill file doesn't specify that). Third, all poligon pours will be just a set of lines. There may be other limitations.
So you CAN do re-export gerber to pcb, but you will get very stripped-down pcb file. In fact, it will be just a set of primitives.

When reverse engineering Gerber's some Gerber software allows you to group flashes and designate them as a component. CAM350 does this, I cannot remember whether Camtastic has this ability (if not its gonna be hard work). Then when you extract the netlist you have actual components. You can use this info to create the base schematic data. import the routing info from the Gerber data as figures and once the netlist and components are read in use these figures as a graphical aid for component placement and routing. Do this quite often for old mil designs where the original company has long gone, but they need to manufacture spares.

From my experience Altium's camtastic doesn't have this feature (at least I didn't see it, no tutorials, no manuals). So when I obtained pcb file, I got nothing but a set of primitives (even texts on silkscreen were just a bunch of lines). I was able to do some simple actions, but surely no further reversed engineering to schematics.
I guess there may be new features in modern versions, or other EDA software that can recreate components. But in general, gerber files are just straightforward descriptors for manufacturing, so extracting circuits from them is kind of magic.

Not so much magic as repetitive work... Its one of those things that can take a long time depending on the the complexity of the design. Multi-layers take forever...