EDIT: Updated part after changes in this thread available in ATmega32 40 pin DIP part submission
I ran that part through a few quick tests. Starting with FritzingCheckPart, then opening the part and trying to work with it, and manual inspection of the files. Here is a quick summary.
The group and id for the breadboard and schematic views do not exist in the svg files.
Fritzing does not handle font size properly when the text uses a size that includes units. It wants things like style="font-size:27.77;", not "font-size:27.77px;" (or font-size="27.77" not font-size="27.77px"). Applies to both breadboard and schematic svgs here.
The breadboard svg includes a connector0 pin and terminal, but that does not exist in the part definition. The connector0terminal rectangle is set with zero width and height, so it probably can not be selected graphically in Inkscape. By convention the connectors are defined starting from 0, and the pin numbers are one greater.
Fritzing converts, but the latest convention is to use black stroke for pcb silkscreen, not white.
The silkscreen block (layer) should be before (earlier in the file) than the copper layers.
The breadboard svg looks good, and seems functional.
The schematic svg looks ok, but could be done as a more logical view, instead of directly matching the chip pinout. There only needs to be a single gnd (typically on the bottom), the VCC connection at the top. The 2 GND pins should be put into a bus in the definition. The pins for the ports are already (mostly) in a blocks, but they could be moved so that the A,B,C,D ports are all together, with the reset of the pins moved above or below the ports. Maybe port B and D on the left, with port C and D on the right. Add blank space on the left or right (if needed) so that PA0 is directly across from PB0, and PC7 is directly across from PD7. This is a logical view, not physical.
The PCB view looks strange. I see a large red rectangle in the middle of the chip outline. Creating a connection to the pins in other views reflects correctly here, but attempting to create a trace to a pin directly on the pcb view, on the top layer, jumps to the center of that red rectangle. The view functionality is broken.
I expect that the top layer problem is because of the way the copper1 and copper0 layers were created in the pcb svg. Typically, THT parts with identical top and bottom layer pads, have all of the connector (circle) elements created once with their ids, then the whole set is wrapped in a group with the copper0 layer id, then THAT group is wrapped in another group with the copper1 layer id. That puts the connectors on both layers. This svg has separate copper0 and copper1 groups with (apparently) identical content, but the connector ids are only in the copper0 group (or bottom layer). To fix this should be as simple as deleting the existing copper1 group with all of its content, then adding the copper1 group around the copper0 group.