How good is HSM Advisor?

[Corey Hampshire]

Let me start with this statement, I have very little Dynamic Milling experience under my belt. The types of parts we have here at work, there is limited opportunity to apply this method. When I see the chance I try and use it and have been successful for the most part. Then I see you guys recommending HSM Advisor and my mind went into chaos.

My methodology for finding feeds and speeds has always been, go with the manufacture's recommendation as a start. Lets say 4340 steel, 1.375 depth of cut is required. Cat 50 Mori mill. Mill chuck, thru air, hydraulic part clamping. I am going to use a 3/4" 7 flute endmill with an ALCRN Base and 38° helix endmill from Garr. https://www.garrtool.com/product-details/?EDP=64186 I pull up their website and it says .003 a tooth and I know from my experience with this material 450 sfm is a pretty good spot for tool life and performance. I set the stepover % to 8%. https://www.garrtool.com/doc/pdf/tech/TECH_VX7_f.pdf 

I then use Mastercam and let it calculate it out for me and run with the speeds and feeds it comes up with when checking the RCTF check box. Matercam comes out with 88.7 IPM and 2292 Rpm. I hit post and go on with my next project.

Then yesterday I downloaded HSM Advisor and was exploring that software. When you guys recommend it, I tend to listen. HSM Advisor mirrors Mastercam's speeds and feeds initially. Then I click on the HSM Checkbox and my head explodes. I can't wrap my head around 4226 rpm and 172.7 ipm. Why the RPM increase? Is this to get the heat out and get the temp into the proper range for the coating? Of course with the RPM increase, the chip load lightens, so we can feed it harder also. 

Am i living life wrong? Should I be spinning my tools faster and running my feeds higher? I know this is a calculator and everything we do is a variable, so it's not plug and play. That said, MRR is way higher than what I came up with in Mastercam and off Garr's website. Am I missing the boat?

[crazy^millman]

2 hours ago, Corey Hampshire said:

Let me start with this statement, I have very little Dynamic Milling experience under my belt. The types of parts we have here at work, there is limited opportunity to apply this method. When I see the chance I try and use it and have been successful for the most part. Then I see you guys recommending HSM Advisor and my mind went into chaos.

My methodology for finding feeds and speeds has always been, go with the manufacture's recommendation as a start. Lets say 4340 steel, 1.375 depth of cut is required. Cat 50 Mori mill. Mill chuck, thru air, hydraulic part clamping. I am going to use a 3/4" 7 flute endmill with an ALCRN Base and 38° helix endmill from Garr. https://www.garrtool.com/product-details/?EDP=64186 I pull up their website and it says .003 a tooth and I know from my experience with this material 450 sfm is a pretty good spot for tool life and performance. I set the stepover % to 8%. https://www.garrtool.com/doc/pdf/tech/TECH_VX7_f.pdf 

I then use Mastercam and let it calculate it out for me and run with the speeds and feeds it comes up with when checking the RCTF check box. Matercam comes out with 88.7 IPM and 2292 Rpm. I hit post and go on with my next project.

Then yesterday I downloaded HSM Advisor and was exploring that software. When you guys recommend it, I tend to listen. HSM Advisor mirrors Mastercam's speeds and feeds initially. Then I click on the HSM Checkbox and my head explodes. I can't wrap my head around 4226 rpm and 172.7 ipm. Why the RPM increase? Is this to get the heat out and get the temp into the proper range for the coating? Of course with the RPM increase, the chip load lightens, so we can feed it harder also. 

Am i living life wrong? Should I be spinning my tools faster and running my feeds higher? I know this is a calculator and everything we do is a variable, so it's not plug and play. That said, MRR is way higher than what I came up with in Mastercam and off Garr's website. Am I missing the boat?

Nothing ventures nothing gained and the idea is yes you getting into the sweet spot of the tool by using what the advisor comes up with.

[#Rekd™]

I always start out with about 75% of what it gives me and then see how the tool/ machine respond and what the part looks like. Then increase from there.

 

[Aaron Eberhard]

The big differences is that the Mastercam RCTF is taking a very limited view of the cross section of tool to engagement angle, and trying to keep that consistent.   HSMAdvisor is looking at the tool stickout (Longer means more deflection of course), # of flutes (more flutes = thicker core = less deflection), coating (big difference in 4340 with TiN vs AlCrN!), angle of the helix (are more flutes in contact at that moment or less?  That affects rigidity and material removal), etc., etc.,   

If you have the machine set up right, it'll help keep you in the proper torque band, too.  Maybe on your spindle if you drop below 2000 RPM, you lose torque, so 1800 RPM = 25 IPM, but 2200 RPM = 45.

One thing I've found is 100% is "normal" high quality setup.  If you're holding things securely in a regular ol' Curt vise with a quality single point/weldon tool holder on a normal Cat40/50 machine that's in good condition, it'll work great.   If you're using an older machine where no one has adjusted the gibs in a while, your tool holders are clapped out and you're often using an ER collet, etc., you'll want to play down at the shallow end of the pool a bit more (75-80%).  If you're using a more modern/well kept machine with a good control, shrinkfits, dovetail workholding, feel free to crank it up into the 120-130% range. 

In my garage, on my robodrill, for example, I generally end up in the 80% range for dynamic roughing.  On a new Okuma that I'm helping out with right now, we're in the 120% range.  

Pay close attention to the Tool Deflection down in the bottom box.  That'll really affect the life of your tool and surface quality. 

Oh, and another handy trick, if you enter a situation where the feedrate or spindle speed is reduced due to safety margins/machine limits, it'll slow down the feed/speed shown as the little green bar below the slider.   If you're trying to figure out what % of a reduction that is, you can type in the number on the RPM or Feed line in the upper right, and it'll set it there so you can match the other:

 

[Corey Hampshire]

Thanks all for the feed back. It looks like I have some experimenting to do. This will be fun and educational I'm sure.

[Matthew Hajicek - Singularity]

With regards to the higher RPM with reduced radial engagement, here's how I think of it.  If you're doing full slotting, the cutting edge is spending 50% of the time heating up in the cut, and 50% cooling down, so you need a low RPM to keep the heat down.  At 50% stepover, it's 25% of the time heating up in the cut, 75% cooling off.  At about 15% stepover, it's 1/8 of the time in the cut, and 7/8 of the time cooling down.  This dramatically reduces the temperature of the cutting edge in the cut.

So you can increase the RPM, which will generate more heat per degree of rotation, until the highest temperature in the cut comes back up to where it would be with your wider engagement.  Then of course increase your feed by the same proportion you increased your RPM, to keep chipload the same. But then with low radial engagement you get to multiply by the chip thinning factor, and then you can really chooch.

[jpatry]

On 10/20/2023 at 6:09 AM, Corey Hampshire said:

I have very little Dynamic Milling experience under my belt. The types of parts we have here at work, there is limited opportunity to apply this method.

I use it on everything, even things I probably shouldn't.

Too bad I can't make it threadmill...

10 hours ago, Matthew Hajicek - Singularity said:

With regards to the higher RPM with reduced radial engagement, here's how I think of it.  If you're doing full slotting, the cutting edge is spending 50% of the time heating up in the cut, and 50% cooling down, so you need a low RPM to keep the heat down.  At 50% stepover, it's 25% of the time heating up in the cut, 75% cooling off.  At about 15% stepover, it's 1/8 of the time in the cut, and 7/8 of the time cooling down.  This dramatically reduces the temperature of the cutting edge in the cut.

This is a good explanation, I think I may even be able to sway the local cultists of the Great Smoothbrained One with it

[#Rekd™]

2 hours ago, jpatry said:

This is a good explanation, I think I may even be able to sway the local cultists of the Great Smoothbrained One with it

I bought my license personally, I can use it wherever I want/ need. Yes my employer should have it but….for $195.00 lifetime it was a no brainer to purchase. 

[amw]

14 hours ago, Matthew Hajicek - Singularity said:

With regards to the higher RPM with reduced radial engagement, here's how I think of it.  If you're doing full slotting, the cutting edge is spending 50% of the time heating up in the cut, and 50% cooling down, so you need a low RPM to keep the heat down.  At 50% stepover, it's 25% of the time heating up in the cut, 75% cooling off.  At about 15% stepover, it's 1/8 of the time in the cut, and 7/8 of the time cooling down.  This dramatically reduces the temperature of the cutting edge in the cut.

Exactly, that's how I look at it too. This also explains why drills run slowest of all, heating up 100% of the time. 

I usually choose an RPM around 1.5X higher then standard feeds/speeds listed for slotting, seems to work ok for us. What do you guys think of this? Sound about right or are you guys usually higher/lower then this? 

[jpatry]

3 hours ago, #Rekd™ said:

I bought my license personally, I can use it wherever I want/ need. Yes my employer should have it but….for $195.00 lifetime it was a no brainer to purchase. 

Oh, I wasn't being naive enough to think I could get them to buy useful tools, I meant convincing them of the use of proper feeds, speeds, depth of cut, and stepover in dynamic milling operations.

 

Okay, their website gave me a giggle...

>>Ideal for more powerful machines such as HAAS

In what universe?

I work in a shop full of Haas, and it's like driving the plastic barbie jeep in the Baja 1000.

[Newbeeee™]

15 hours ago, jpatry said:

In what universe?

I work in a shop full of Haas, and it's like driving the plastic barbie jeep in the Baja 1000.

Yehbut in my world, at least you'd look good....

[Newbeeee™]

On 10/20/2023 at 4:28 PM, Aaron Eberhard said:

The big differences is that the Mastercam RCTF is taking a very limited view of the cross section of tool to engagement angle, and trying to keep that consistent.   HSMAdvisor is looking at the tool stickout (Longer means more deflection of course), # of flutes (more flutes = thicker core = less deflection), coating (big difference in 4340 with TiN vs AlCrN!), angle of the helix (are more flutes in contact at that moment or less?  That affects rigidity and material removal), etc., etc.,   

If you have the machine set up right, it'll help keep you in the proper torque band, too.  Maybe on your spindle if you drop below 2000 RPM, you lose torque, so 1800 RPM = 25 IPM, but 2200 RPM = 45.

One thing I've found is 100% is "normal" high quality setup.  If you're holding things securely in a regular ol' Curt vise with a quality single point/weldon tool holder on a normal Cat40/50 machine that's in good condition, it'll work great.   If you're using an older machine where no one has adjusted the gibs in a while, your tool holders are clapped out and you're often using an ER collet, etc., you'll want to play down at the shallow end of the pool a bit more (75-80%).  If you're using a more modern/well kept machine with a good control, shrinkfits, dovetail workholding, feel free to crank it up into the 120-130% range. 

In my garage, on my robodrill, for example, I generally end up in the 80% range for dynamic roughing.  On a new Okuma that I'm helping out with right now, we're in the 120% range.  

Pay close attention to the Tool Deflection down in the bottom box.  That'll really affect the life of your tool and surface quality. 

Oh, and another handy trick, if you enter a situation where the feedrate or spindle speed is reduced due to safety margins/machine limits, it'll slow down the feed/speed shown as the little green bar below the slider.   If you're trying to figure out what % of a reduction that is, you can type in the number on the RPM or Feed line in the upper right, and it'll set it there so you can match the other:

 

I have a notepad doc with tool diameters, type/make, stickout, holder and material as default go-to's for what has previously worked (well). But if I was still doing "it", I'd buy this.

Yours is the best explanation I've ever read on this. For what it does compared to the Mcam RCTF (disclaimer - which I never used), if I was CNC i'd "buy Bob" and properly integrate into Mcam....

 

 

[neurosis]

On 10/22/2023 at 5:55 AM, #Rekd™ said:

I bought my license personally, I can use it wherever I want/ need. Yes my employer should have it but….for $195.00 lifetime it was a no brainer to purchase. 

I did the same.

I liked the idea of being able to take it with me if I ever needed to relocate. 

[JoshC]

On 10/23/2023 at 3:20 AM, Newbeeee™ said:

I have a notepad doc with tool diameters, type/make, stickout, holder and material as default go-to's for what has previously worked (well). But if I was still doing "it", I'd buy this.

Yours is the best explanation I've ever read on this. For what it does compared to the Mcam RCTF (disclaimer - which I never used), if I was CNC i'd "buy Bob" and properly integrate into Mcam....

 

 

i seen bob bashing mastercam on one of his blogs once, or at least making it seem like something else was superior to mastercam when it was all his opinions and nothing factual that i read,  so i lost some interest in his products...

was a while back and not sure if he still has it up or not but kindof ticket me off because he was incorrect on his opinions. if he has a good product feel free to use it if yall want to but he rubbed me the wrong way with that post he has up, ill see if i can track it down at all

Edit: Sorry im talking about G-wizard not HSM advisor,  just noticed you are all talking about hsm advisor so nevermind and found the article here https://www.cnccookbook.com/cnccookbook-2023-cam-software-survey-whats-the-best-cam/ , very opinion based article and states at the top somewhere that fusion 360 is the overall market leader and that mastercam bobcad and hsmworks are all down on share lol whatever that means, so we are grouped in with BOBCAD and fusion 360 is better than mastercam is just laughable 

[Newbeeee™]

16 minutes ago, JoshC said:

i seen bob bashing mastercam on one of his blogs once, or at least making it seem like something else was superior to mastercam when it was all his opinions and nothing factual that i read,  so i lost some interest in his products...

was a while back and not sure if he still has it up or not but kindof ticket me off because he was incorrect on his opinions. if he has a good product feel free to use it if yall want to but he rubbed me the wrong way with that post he has up, ill see if i can track it down at all

Edit: Sorry im talking about G-wizard not HSM advisor,  just noticed you are all talking about hsm advisor so nevermind and found the article here https://www.cnccookbook.com/cnccookbook-2023-cam-software-survey-whats-the-best-cam/ , very opinion based article and states at the top somewhere that fusion 360 is the overall market leader and that mastercam bobcad and hsmworks are all down on share lol whatever that means, so we are grouped in with BOBCAD and fusion 360 is better than mastercam is just laughable 

Josh - you'd be great in politics - I'd vote for you

Edit:- my bad, I got the products and owners/writers mixed up (with name of Bob). Same comment though, buy HSM and integrate it!

 

[Aaron Eberhard]

1 hour ago, JoshC said:

i seen bob bashing mastercam on one of his blogs once, or at least making it seem like something else was superior to mastercam when it was all his opinions and nothing factual that i read,  so i lost some interest in his products...

was a while back and not sure if he still has it up or not but kindof ticket me off because he was incorrect on his opinions. if he has a good product feel free to use it if yall want to but he rubbed me the wrong way with that post he has up, ill see if i can track it down at all

Edit: Sorry im talking about G-wizard not HSM advisor,  just noticed you are all talking about hsm advisor so nevermind and found the article here https://www.cnccookbook.com/cnccookbook-2023-cam-software-survey-whats-the-best-cam/ , very opinion based article and states at the top somewhere that fusion 360 is the overall market leader and that mastercam bobcad and hsmworks are all down on share lol whatever that means, so we are grouped in with BOBCAD and fusion 360 is better than mastercam is just laughable 

Yeah, Eldar is genius behind HSM works.   In my opinion-based rating, HSM is world ahead of GWizard, at least it was when I evaluated it a while ago.

And the problem with surveys like this is:  How did you reach your test audience? 

Is the survey you're hearing about representative of people who still have a land-line and answer an unknown number's call?   Yes?  Well, then, I'm questioning the results...

[gcode]

5 minutes ago, Aaron Eberhard said:

Is the survey you're hearing about representative of people who still have a land-line and answer an unknown number's call?   Yes? 

I evaluated gwiz a few years ago

I never bought it and never unsubscribed from his email list

He sends out his survey to his email list annually..  I've never participated in that either.

 

[Aaron Eberhard]

18 hours ago, gcode said:

He sends out his survey to his email list annually..  I've never participated in that either.

 

Well, I guess we know who's responsible then... 

 

[Corey Hampshire]

I used HSM Advisor yesterday on a project I am working on. I have a 25mm 4 flute Sandvik indexable screwed onto a heavy metal shank that I am using to side mill the cheeks on a crankshaft with. Normally I would run it at .004 a tooth and 475ish sfm. That is where I started at. It worked out to be 40 IPM and 1900 RPM. 

This particular crank is a 6 cylinder so I had 6 pins to play on. HSM Advisor suggested 76 IPM and 2100 RPM. I took the advice offered here and started at my normal speed and feed and adjusted up each pin. I ended up at 72 IPM and 2100 RPM. The only reason I didn't get to 76 like HSM Advisor suggested was that I ran out of pins. I will try it on the next crank.

Of course surface finish suffered as I increased feed rate, as expected, but for what I am doing, it doesn't matter on this op. I was able to take a solid 4 mins of cycle time out, which will work out to over 24 mins a crank from my baseline. Time is money as we all know. 24 mins times 30 cranks and HSM is priceless. This is just one op. It has paid for itself already and stuck money back into the companies pocket.

This has really got me thinking about my approach to, well, everything. There are other projects that I want to go back and re-apply this on now. I have a dynamic milling project I am probably going to do today or tomorrow in a horizontal cat 45 mill so I will get the chance to play more on HSM Advisor then.

Thank you guys for the info, feed back and help. This place is awesome and I read here everyday. I always seem to pick up something new and it makes me think daily. 

[rchipper]

On 10/22/2023 at 5:55 AM, #Rekd™ said:

I bought my license personally, I can use it wherever I want/ need. Yes my employer should have it but….for $195.00 lifetime it was a no brainer to purchase. 

May I ask which license you purchased?

Ah, I see only 1 license for $195.00. Sorry.