Dynamic milling

[alloutmx]

Im trying to cut a portion from a block, picture a square split into 4 quadrants, and im try to only mill the upper right quadrant out. what is the proper Dynamic milling function, and entry method. I want to engage from the outside right corner, taking a few air cuts as possible. I can send mcx file to you if youd like to help. Thank you in advance...im having a f of a time

EMASTERCAMHELP.MCX-6

[Guest]

Here's a suggestion

 

Trying to attach an mcx-7 file and the forum keeps telling me I'm not allowed to upload this kind of file???

 

huh?

[alloutmx]

what path did you use? Im having a heck of a time getting the cutter to start from the outside corner

[Guest]

That a Dynamic Core

[alloutmx]

thank you for your help...why is it neccessary to use an avoidance chain?

this is where i am at now...

EMASTERCAMHELP.MCX-6

[Guest]

I used the avoidance because in using the Dynamic Core and needing to start outside, I need some kind of avoidance chain.

[alloutmx]

Im glad i have a result, but im still not sure how i got there...why does it need an avoidance boundry when i gave it an entry point? seems like if you give it an entry point that it would start outside your stock reguardless of the avoidance boundry. So i guess i still have some questions as to why, but you definitly got me there JP

[MotorCityMinion]

You don't necessarily need an entry point. On the cut parameters page, there is a approach distance setting and a tab with with a drop down menu that allows you select a zone in which to approach the part. This works in combination with the Machining and Avoidance chains to determine how to enter the cut.

 

You need to change up your train of thought here. This may sound goofy but don't think of it as a part. Normally in a 2D contour we select the actual part geometry we want to cut. With dynamic, the perspective changes how we look at the part and the avoidance region becomes our actual machining geometry, with the machining region only representing the raw stock to cut away.

 

The first chain, the machining region in red, represents the stock we need to remove, not necessarily the part, and is the target cut area. This can be any shape to accommodate the raw material at hand or our stock removal requirements, and usually contains some, if not all of the part geometry. It does not have to match your part geometry either. With core milling, the cutter can and will go around the outside of this chain and is only limited by the avoidance region. See picture.

 

The second chain, the avoidance region in light blue, not only represents the part but the area we want to stay out of. Think of it as an electric fence we can't touch by .02, stock to leave. Notice in JP's example how the avoidance region goes beyond the machining region. Only three elements of that region actually represent part geometry. This tells Mastercam to stay out of this yard and will be used to control the cutter path. This chain shape can be almost anything willy nilly as long as some of the geometry represents where not to cut, which normally contains some if not all finished part geometry. We could have actually used the rest of the actual part geometry to define the avoidance region. Mastercam looks at both chains and knows that there is nothing to the left of the avoidance region that requires cutting and stays out of that neighborhood.

 

OK, so I go grab a fresh cup o joe, come back and find my beagle standing on my desk finishing off my doughnut and she has one paw on the mouse. (Yah, I've got too much time on my hands). Now look at my chain geometry. I hit regen and woah, I have a very similar tool path. Look at the picture below. JP's on the left, mine on the right. Take notice of how the avoidance chain influenced the entry and produced an arc leading in. Very cool. The point is, these chaining options are very flexible and limitless. Almost anything will work once you get your head in the right place.

 

I hope all this gibberish helps somebody out, MCM.

[alloutmx]

awesome...im going to read it 6 or 7 teen more times to make sure im getting it all, but it makes more sense to me know for sure.

[alloutmx]

thanks for your help fellas!

 

[MotorCityMinion]

Bump up the back feed rate. Late models Haas = 400. ipm, Older machine = 300. ipm. It looks like the part is already squared. Make the machine region chain exactly the same as the part boundary and you'll cut on that first pass. As for the ZIGZAG cutting motion, that can be detrimental to tool life, especially in tool steels. Two axial Z passes? Bump up the radial step over to 12%, climb cut only, you'll make up the lost ZIGZAG time and increase tool life. Start in the top left as this will increase the length of cut and actual engagement time, reduce the cycle time and reduce the tool path size as well as reduce the additional wear incurred by repeatedly entering the raw material. Chips should look straw colored to purple.

[alloutmx]

In the video... Special thanks to the HSM Advisor and the SolidWorks cam guide???

 

Bump up the back feed rate. Late models Haas = 400. ipm, Older machine = 300. ipm. It looks like the part is already squared. Make the machine region chain exactly the same as the part boundary and you'll cut on that first pass. As for the ZIGZAG cutting motion, that can be detrimental to tool life, especially in tool steels. Two axial Z passes? Bump up the radial step over to 12%, climb cut only, you'll make up the lost ZIGZAG time and increase tool life. Chips should look straw colored to purple. Dat B how we do it.

 

i saw the zig zag in a video this guy showed me last night(solidworkscam guy from practical machinist forum) and HSM advisor is a chip thinning calc that i guy i met on that same forum developed and sent me.

 

I realize the zig zag is pretty awful, but man it sure was cool!

 

Total depth was 1.125 and i dont think we have anything in .500" dia that would cut that deep one pass...but maybe...

 

Step over was .035 per pass and chips were purple like u say...next video i give you a shout out too. hope your not mad bro...but we just met ya know?

 

GO READ THE COMMENTS..I PLUGGED YA

[alloutmx]

also...im not sure my machine can handle backfed that fast...it starts to wash out after 100ipm....1996 haas vf1. i gotta kill this machine and maybe they give me something better...but its far better than the bridgeport i use to make tooling on!

[MotorCityMinion]

You should be fine on that machine. I've done quite a bit of this type work on a 98" vf4 with only 15 hp. Who knows though, your machine may have been beat to death already but these tool paths excel on terrible machines. Make sure your getting arcs in your tool path, use the arc filter for smoother motion if need be.

 

"next video i give you a shout out too. hope your not mad bro...but we just met ya know?"

 

LOL, no need, it's all good. Keep up the good work. Pretty soon you'll be looking at everything and saying to yourself "Where can I use Dynamic milling?" on every job. I edited my last reply omit the stupid comments.

 

"Total depth was 1.125 and i dont think we have anything in .500" dia that would cut that deep one pass...but maybe..."

 

I've gone that route on the older Haas with long e-mills and the tool life sucked. I had to go down as low as 8% step over at full depth to keep things manageable. Going around corners on that first pass can wreak havoc as radial engagement can get heavy in these areas. Snapped a few tools in my time as well.

 

I have about 6 different speed and feed calculators and they all churn out something different. I've also studied the competition's know how with regards to adaptive clearing and there's a ton of good info to be had.

[alloutmx]

You should be fine on that machine. I've done quite a bit of this type work on a 98" vf4 with only 15 hp. Who knows though, your machine may have been beat to death already but these tool paths excel on terrible machines. Make sure your getting arcs in your tool path, use the arc filter for smoother motion if need be.

 

"...AUSTRIA?!? welll then...gooday mate...lets put another shriiimp on tha bahbee"

 

so would you suggest 300 ipm when i get into cutting these paths in aluminum? Ive been toying with these paths for a few years, but never at these speeds. generally use standard feeds and speeds at heavier DOC

[MotorCityMinion]

That picture I use was a goof. Inspiration: One day my kid came home with a bad hair cut just like that. I cant remember but I think he says that in the movie. I need to change that picture.

 

I've gone about 220. IPM with a low quality 3/8 emill x .70dp. in Aluminum no problem on the 98 VF4. Biggest issue was getting the chips out of the way.

 

IMO, that first picture that JP posted represents the smoothest motion and is how I would approach it. Larger tool dia. perhaps but the technique was spot on.

[Rotary Ninja]

I am running a VF2. I am unsure what year it is but it will only accept a 300 IPM feedrate. In 6061 I run a 1/2" endmill with around a 1-1/2" DOC with a .050" stepover at 200 IPM feed and 11000 RPM when using the Dynamic stuff. I have my default back feedrates set to 300 IPM. When you have a large pocket these toolpaths are really impressive.

[alloutmx]

I am running a VF2. I am unsure what year it is but it will only accept a 300 IPM feedrate. In 6061 I run a 1/2" endmill with around a 1-1/2" DOC with a .050" stepover at 200 IPM feed and 11000 RPM when using the Dynamic stuff. I have my default back feedrates set to 300 IPM. When you have a large pocket these toolpaths are really impressive.

we've got a couple vf2s here that i keep raggin the boys to give me or trade me...my spindle is 7000 max, and i tried 200ipm once on accident probalby 4 yrs ago when i didnt have a clue(not that i do now) and it turned an arc in a 45dg angle...it didnt know wtf was going on. ill try it again tho.

[Rotary Ninja]

What is your corner rounding setting set at?

[alloutmx]

i dont see the corner rounding selection for this type of [path. not saying it isnt there...just that i dont see it

[Rstewart]

Corner rounding in the machine settings....

 

Can remember which # it is, but just scroll through the setting menu on your controller and set it to like .01

[Rotary Ninja]

Setting 85 in the Haas control on the machine. We have ours set to .005". It does pretty good and the only time I see anything on the part is when we have an external corner rad to create an edge break on sharp corners.