The short answer is yes, unless you adjust parameters, it will be slower, so you will need to change how you set your cutting conditions.
With the same parameters, the HSM toolpath (constant load) will be slower than the roughing toolpaths for volume milling. This is because it spends more time gently entering a cut, repositioning, and adjusting step-over to keep cutter engagement constant. Parameters shouldn't be similar between the two. This HSM toolpath is much more sophisticated than the relatively simple algorithm used in conventional tool paths. It allows much more aggressive cuts and allows you to get better life out of the cutter.
In your volume roughing toolpath example, it varies roughly from 90 degrees cutter engagement to 180 degrees. Most likely, you will set the feed rate and depth of cut to the 180 degree condition, to avoid breakage and chatter. That means that everywhere the 90 degree engagement prevails, you are going too slow. In addition, the 180 degree engagement is not ideal for tool wear, since it rubs before cutting. In your example, you have a 12mm end mill with a 40mm length of cut. However, you only take approximately 1 mm depth per pass, which means that the most of the cutting edge of the tool is not being used, and it will be worn out long before its time.
I would start the HSM parameters by going the full depth of your 20mm depth. I would then adjust stepover to 5-10% or so of the diameter. If all is good, you can increase that until you get chatter or breakage or back off if you think that's too much, The feedrates, due to chip thinning, can be increased as well. The nice part is that once it starts off good, you don't as often have to worry about a surprise chatter squeal or overload. You might look for a good online calculator. The HSM toolpaths are just much smarter in other ways too, and I always reach for them first.
