What's new
What's new

First try using HSM toolpath

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
So this week i was giving a try at Fusion 360 cam. We had a order of 64 piece to do so it was a good timing to try these HSM toolpath

here is a quick video of 1 of the roughing toolpath that i make
https://www.youtube.com/watch?v=Tf6_GcMeWdo&feature=youtu.be

I know the video quality is not the best but i film this with a tablet so sorry about that.

here is the spec of the cut

Material: SS 361L
size 4.750 long 1.5 width 0.500 height
Endmill: Niagara STR440 Stabilizer HT
5000 RPM
110 IPM
0.400 DOC
0.038 WOC

i know its not the most impressiv video out threre but i did this on a small tool room mill similar to a haas TM1 So here is the spec of the machine.

Mansford VM1000 Fagor 8055 I MC control
7.5 hp direct drive
454 IPM rapid travel
8000 RPM
Carrousel tool changer 10 position
around 8000 pounds

Here is a picture of the finish part
gripper.jpg

Finish part is 4.439x 1.280

the part also have 2 other feature (slot and circular) that i did with HSM strategie. both were using a 1/4 endmill at 7100 RPM 58 IPM 0.400 DOC 0.025 WOC. Both endmill (3/8 and 1/4) were doing the roughing/finishing of the piece (thanks to my 10 position carrousel) they also both of them do the whole 64 piece batch and were withing 0.001 from the first to the last piece so they hold up well.

I know its not the best toolpath or optimize program out there so every usefull information is the welcomre to get better in the futur.

I would also like to say thanks to zero_divide for the help he gave me with the speed/feed and after using is HSMadvisor i suggest to everyone to give it a try its realy worth it.

Sébastien
 

pgmrmike

Cast Iron
Joined
Jun 24, 2010
Location
Plantersville, TX
Awesome. Just ran my first HSM job a couple of weeks ago but I was much more conservative than you were. Gotta admit, when I hit the button I was scared! Ran a 12pc order and when I was done the EM was still sharp, no noticable wear, 4140HT, SGS Z Carb.
 

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
Awesome. Just ran my first HSM job a couple of weeks ago but I was much more conservative than you were. Gotta admit, when I hit the button I was scared! Ran a 12pc order and when I was done the EM was still sharp, no noticable wear, 4140HT, SGS Z Carb.
On the first part i was scare to since im use to program with my convertational control that got like 2 or 3 safety move before entering the cut and this one is strait into buisness no time lost so i was like holy.... But i also had alot of faith in my toolpath and the speed feed. I was more worried about the 0.090 thick material i was hanging on into the vise ive read alot about hsm toolpath pulling part up or endmill out of holder so i was hoping it was enought and it did.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
I was more worried about the 0.090 thick material i was hanging on into the vise ive read alot about hsm toolpath pulling part up or endmill out of holder so i was hoping it was enought and it did.

If you are holding .090" and the material is decent (not rounded over on the corners), that is generally enough if using a 3/8 or 1/2" endmill.

But, if the material you have sucks, or you have as little as .060" to hold on to, you should get a few sets of these: Mitee-Bite Products Co. - TalonGrip<sup>™</sup>

There are other companies that make jaws that can hold onto a similar amount of stock, so shop around. These are the ones we use, and regularly hold onto .100" or less (.06" minimum)
 

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
If you are holding .090" and the material is decent (not rounded over on the corners), that is generally enough if using a 3/8 or 1/2" endmill.

But, if the material you have sucks, or you have as little as .060" to hold on to, you should get a few sets of these: Mitee-Bite Products Co. - TalonGrip<sup>™</sup>

There are other companies that make jaws that can hold onto a similar amount of stock, so shop around. These are the ones we use, and regularly hold onto .100" or less (.06" minimum)
Yeah it was mechanical flat bar its a bit more expensive but you get 2 strait edge to hold on and save alot of time at the end.
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
On the first part i was scare to since im use to program with my convertational control that got like 2 or 3 safety move before entering the cut and this one is strait into buisness no time lost so i was like holy.... But i also had alot of faith in my toolpath and the speed feed. I was more worried about the 0.090 thick material i was hanging on into the vise ive read alot about hsm toolpath pulling part up or endmill out of holder so i was hoping it was enought and it did.

Thanks for mentioning my software!
I myself get scared sometimes. Especially when running > 2x depth for cut at high feedrates.
Using a lot of experience, trial and error and good observational skills it is possible to program efficient HSM toolpths, but I, for one, break tooling almost excursively when trying to guesstimate cutting parameters in my head, instead of just figuring what WILL work for sure in a couple of mouse clicks.

It is OK to run DRY with free-machining or hardened stainless steels/ But the softer, gummy ones tend to stick to cutting edge no matter what you do and coolant is pretty much the only option.

Also you have to make sure chips clear the work area, as they easily chip the cutting edge when being recut in HSM-type toolpath.
 

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
Thanks for mentioning my software!
I myself get scared sometimes. Especially when running > 2x depth for cut at high feedrates.
Using a lot of experience, trial and error and good observational skills it is possible to program efficient HSM toolpths, but I, for one, break tooling almost excursively when trying to guesstimate cutting parameters in my head, instead of just figuring what WILL work for sure in a couple of mouse clicks.

It is OK to run DRY with free-machining or hardened stainless steels/ But the softer, gummy ones tend to stick to cutting edge no matter what you do and coolant is pretty much the only option.

Also you have to make sure chips clear the work area, as they easily chip the cutting edge when being recut in HSM-type toolpath.

i did another part today my boss told me we needed them in a hurry and that he dont mind if we burn a endmill doing the 40 piece run. so i put a 1/2 endmill 7100 rpm 140 ipm i stack 4 sheet metal piece of 0.090 thick and put a hole 5 5/8 inch in them every run took under 3 min for 4 part done. that thing was scary too. but man it is fun. I like when im at work with a big smile alone in the corner of the shop with the sound pleasure comming off the machine :P
 

SR910

Plastic
Joined
Nov 2, 2014
How did you go with the post for fusion? I have a few machines with anilam controllers and being less popular I don't want to be stuck trying to build my own posts.
 

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
Well at first the generic post didnt work with my control. Ive watch over the forum and find 4 other different post and finally one on them work. I had to change a couple of thing by hand that took 2 min but im using it in free trial and when i buy it im going to work towards modifing those little things and everything will be fine i think.
 

Atomkinder

Titanium
Joined
May 8, 2012
Location
Mid-Iowa, USA
How did you go with the post for fusion? I have a few machines with anilam controllers and being less popular I don't want to be stuck trying to build my own posts.

The Fusion/HSMWorks post guys are extremely helpful. I've had them make post changes twice and got them in just a couple days each time. You just mark up a posted file with notes about what you want where and they fix it right up. I'm sure they would even do it during a trial.
 

Krovvax

Hot Rolled
Joined
Mar 5, 2012
Location
Quebec, Canada
The Fusion/HSMWorks post guys are extremely helpful. I've had them make post changes twice and got them in just a couple days each time. You just mark up a posted file with notes about what you want where and they fix it right up. I'm sure they would even do it during a trial.
Yeah well for some minor fix like these (turning coolant on, switching g54 to g159n20, removing the m6 on the tool change since i only need t2 to change tool) is not a big deal so i dont want to bother them until i buy it. I actually download it to get my boss to see the potential vs the conversational control since they dont know anything about machining the best way to make them change their mind is to show them real number so they save money.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
Just from what I read here on the forum. The increased surface footage increases the heat at the cutting edge, and running coolant on it leads to thermal cracking.

Shouldn't most of the heat stay in the chip? To be honest I've never felt my endmill after cutting an HSM toolpath, but I have felt my part and it's barely warm to the touch.
 








 
Top