[BNX]

Ok got question. For this type of work I am doing with a.375, 4 v. flute, GWizard tells me to run something like this for manufacture's spec.


GWizard


or this one



Here another one I did. Having the program opt for the depth, rpm, feed and locking only the width.

[BNX]

Ok another sample. I'm not sure if I am heading the right directions.

This time with their .25 4 v. flute. I guess the machine can't reach 500 sfm so this is what I got with GWizard.


This is the max I could get.


I don't feel comfortable running that fast so what do I do to adjust it? I am just locking the max rpm like this. I don't think I am doing this right.


I think I missing something. Can't figure it out. Am I reading the manufacture's spec wrong?

[SCzEngrgGroup]

You're getting wacky numbers because you're setting crazy small cut depths. Are you confusing chipload with cut depth? Set cut depth to something reasonable, like 1/2 the tool diameter, set cut width to the tool diameter, and let GWizard handle *everything* else. It's not necessary to look at the tool manufacturers data, or for you to manually enter any other numbers (other than the machines RPM, feed and power limits) - that is what GWizard is for, and the numbers it generates will be plenty good enough for your needs.

Regards,
Ray L.

[BNX]

You're getting wacky numbers because you're setting crazy small cut depths. Are you confusing chipload with cut depth? Set cut depth to something reasonable, like 1/2 the tool diameter, set cut width to the tool diameter, and let GWizard handle *everything* else. It's not necessary to look at the tool manufacturers data, or for you to manually enter any other numbers (other than the machines RPM, feed and power limits) - that is what GWizard is for, and the numbers it generates will be plenty good enough for your needs.

Regards,
Ray L.

I'll try that. I did some crazy stuff when I first used GWizard. I was using a 1/4 2 flute, I think about 30ipm at probably 4800 or so. It snapped so fast I never found the mill. I been running it slow again without the wizard, lol.

I went with GWizard again when I got my new Tormach 17mm end mill. I broke the damn thing on my first run, 6061. I left GWizard again.

Thanks for the pointer.

[BAMCNC.COM]

FSWizard err... HSM Advisor would be in your best interest

[BNX]

FSWizard err... HSM Advisor would be in your best interest

Avast keeps blocking the file. When I turn off firewall and security, it's fine. When I turn it back on it deletes the file again.

[btu44]

If I may offer this, here's my the way I select cutting parameters for my PCNC1100.

I use a freeware calculator called ME Consultant 2.0. It's on a few download sites when I Google it. It has a DOS feel to it, so I don't think viruses are an issue.

So for me, there are a few constants I like to use. I'll use the published chip load for the cutter and material I'm using. I may adjust it down a little if it seems too heavy. Typically in aluminum with carbide, .004" for a 1/2" EM, .002" for a 3/8, .001" for a 1/4".

When I'm roughing aluminum as fast as possible, I usually use a 1/2" end mill at 3200 RPM. This seems to be the RPM were motor torque really starts to fall. I think it is more important to be at near peak spindle torque than trying to meet published SFM. When I'm using a 3/8 end mill, 3800 RPM works well.

When rough contouring I'll use 30% of the tool diameter for the WoC. And for slotting, well WoC is hard to adjust.

So if I have a new end mill that I want to setup a feed and speed for, here's how I do it.

Using ME Consultant, I'll enter the stock material, select carbide end mill, enter the end mill diameter and the number of flutes.
Next I'll enter the RPM Limit for the cutter I'm using, example 3200 for a 1/2" EM. This way I will not get a calculation above this RPM.
For WoC I'll either enter 30 or 100% of the tools diameter.
Then lastly I'll adjust the DoC to a calculated .9 horsepower. This gets me pretty close for a starting point.
Then I'll do some test cuts on some rem material. Better to break an end mill than scrap a parts and break an end mill. I'll look for the spindle bogging down, tool pull out and chatter. If the spindle bogs or the tool pulls out, I'll decrease the depth of cut. If there excessive chatter after adjusting the DoC, I'll adjust the feed and RPM down to maintain the same chip load.
A variable to this is a very deep slot or pocket. The stock coolant system on the PCNC1100 is not so good at flushing out chips. Sometimes I'll back off the DoC to control the amount of chips being produced.

So I know there are many techniques for feeds and speeds. I worked with a guy that in aluminum it was 3000 RPM, 30 IPM for every end mill...he liked it simple. This is just away that is working well for me.

Barry

[BAMCNC.COM]

Avast keeps blocking the file. When I turn off firewall and security, it's fine. When I turn it back on it deletes the file again.

Use online version.

[waltpermenter]

Use online version.

kinda moots your whole argument about not using gwizard because it has to connect to the internet once in a while now don't it.

[BAMCNC.COM]

Do you have a Smart Phone? The mobile version is great

[zero_divide]

Avast keeps blocking the file. When I turn off firewall and security, it's fine. When I turn it back on it deletes the file again.

I filed a false positive claim with avast.
Hopefully they will fix it next time it updates.
Ironic considering it never connects to the internet.

Btw. Unlike other calcs there is absolutely no way you can snap an endmill or drill with HSMAdvisor.
It automatically analyzes each calculation against deflection and torque and limits the feedrate. And when it can't it bugs you with warnings
Even though FSWizard gives identical results it does not perform those checks.

[BAMCNC.COM]

Good to know! Thanks Zero