Couple quick questions on programming paths and feed rates

[honeybunches]

Q1, For simplicity, lets consider a round part out of a square billet. If you program multi passes around the profile of the part, you will end up cutting a lot of air. In stead, I usually end up creating extra geometry to trim the excess material off. However, the machine tool is very sensitive to radial tool engagement. I would like to, for example, maintain a 45% engagement while reducing how much air gets cut.

 

Is there a good solution for this?

 

I am running X2MR2.

 

 

Q2, Example, I create 4 chains but one of them needs a slightly reduced feedrate so I right click the chain in the geometry tab and select "adjust at point" and adjust the feed. However, when it posts out, the feedrate has not been altered. Am I missing a page here?

[chopsley]

Q1 - Sounds like 2d High speed core milling might give you what you are looking for.

 

Q2 - Can't help with that one. I'm sure someone else will.

 

[Dan@home]

Q1...If I am not mistaking X2 doesn't have 2D HS. You can try the 3d HS and mess with steep/shallow and depth of cuts.

 

Q2...If you select the toolpath you want to change or edit. Then right click and select the (toolpath editor) this gives you way more options than change at point. After you are done the op will be locked. If you want to go back to original TP, unlock and regenerate.

[chopsley]

I thought X2 had the HS core milling but I could be and am probably wrong. What features go with what versions are just becoming a blur to me. Sorry bout dat. Daily I have to offset lines to make facing tool path geo because I cannot get MC to start at the upper right hand corner of the part which is a must for what I am doing. Some day perhaps.

[Dan@home]

chopsley, not 2D.

[honeybunches]

Colin, the reason for programming heavier DOCs is this machine is limited in rpm and feed. Anything much over 100ipm and it will overshoot for sure. If I combine light cuts with slow xxxx machining, it will take forever.

 

I am open for suggestions. In some stuff, I am actually at 60% engagement and not able to feed much. Only .002 per tooth with a 3/4 tool. This is Al. My axial DOC is .500. I tried .600 and the machine could not do it. I am certainly open to ideas. Possibly reducing my WOC, increasing my DOC and feed might prove a better solution.

 

Also, I have never tried the trim toolpaths, is this specifically designed for such work?

[honeybunches]

ON Q2, I checked that the filter was not on. The Infinite lookahead was and turned it off but no change in code. Still posting to same feedrate.

[honeybunches]

I checked the NCI file and feeds do not change. Has to be a settings issue. Just not sure what yet.

[honeybunches]

I did some playing outside my comfort zone for new paths. It just really seems that MC needs to be able to recognize my stock dims and create paths based on that. Rapid over to the next cut when it is cutting air, etc. I have not found a path yet that I like in X2. Does X4 have better solutions for this? Am I missing a chapter in path creation? I do not do HSM machining much or surfacing. Just looking for some smarter roughing paths.

[kunfuzed]

quote:

---

Does X4 have better solutions for this?

---

Yes. 2d Highspeed Core Mill. My favorit for what you are doing is 2d Highsped Dynamic Milling with Core Mill Passes turned on.

 

You should be able to get your HST Core Roughing to work with some playing around. What I don't like about the 2d and 3d core roghing paths is the first cut pass on the perimeter of the stock is a really wimpy one that jumps back and fourth. If my stepover is at .375 it might just take a .05 bite. Any ideas on that?

[Zoober]

Try rest mill. make an STL of your stock, and zoom. It knows where the stock is and isn't. And you can hug the part as you move about.

[Jayson Kramer]

Viper1, hay for old times want to share your file with me so I can see what you have and give some ideas?

[Programinator]

I have issues with change at point as well. I can get it to post out different feedrates but it never seems to put them in the correct spot for some reason. For example if i want to slow down feed in a corner only and then speed back up. I go to toolpath right click, change at point, select corner rad, check feedrate and change, click ok, select entity after corner rad, change back to original feed, and so on.....

 

post out and somtimes it works but most times it puts feed change on wrong blocks of code. Sometimes it does not change back to original feedrate. Sometimes i get an error that says the second feedrate will be ignored.

 

Most of the time on the rare occation that i need to change the feed i end up getting frustrated just manually editing code which bugs me. I dont like doing that because next time i may forget to do it.

 

Anyone have any enlightenment on this?

[Programinator]

Just tried the toolpath editor for my situation and it just works like i want. Im going to start using that instead of change at point. Never even knew it existed until today.

[allena]

In X2 there is trim toolpath function. draw a rectangle "border" a little bigger than the stock,program 4 quadurants of the circle. then use trim toolpath to trim away any movement outside the rectange border

[Jayson Kramer]

Allena, this has been around in MC for along time. I used to trim tool-paths back in V6.1a. it can be a great tool if used right.

 

Programintor, you will like the control.

 

It is funny, as I see this almost daily at times the tools that even people that have used it for years do not know that Mastercam can do. this is a very powerful tool for us. You just read here on this forum like you folks in this Post and still learn something new.

As a over 20 year user dealer ,teach support and teacher of .I still do not know everything as every new release gives us more and more.

CNC has come so far and there are allot of people have know idea what it takes and really how much that all the great people including the two Ceo's listen to what you all say here.

 

If you think about the issues that are alwas pointed out on this forum think of how many non issues that make the software what it is today. and how hard it is to keep all this in order. From my point this is unbelievable.

 

JM2C

[Programinator]

quote:

---

It is funny, as I see this almost daily at times the tools that even people that have used it for years do not know that Mastercam can do.

---

That is so true Jay. Thats why i dont let a day go by without at least browsing emastercam for a few min. What a blessing this site has been for me. If i was an employer who had a programmer as a employee i would tell them to make sure they take advantage of this site on company time. Thats how powerful a tool it can be with all the talented people like you Jay who live here.

 

The company manual would say "All Programmers must go to www.emastercam.com during the last 15 min of every work day"

 

Yesturday when i learned about the toolpath editor i was so happy. I even called my wife to tell her. I said to her guess what. She said what! I said i figured something out in mastercam that i been fighting with for some time now! she said ok with not much enthusiasum. I said sorry i just wanted to tell someone.

 

So to get a better reaction i called a buddy of mine and told him about it. I said how do you change feed rates in a toolpath without manually changing it after posting. he said oh you just go to change at point. I said how does it work. He said well sometimes it puts the feed rate in the wrong place. Then i said dude......toolpath editor....use it. He loved it and i loved sharing something i learned.

 

So i guess the point is that the emastercam family made my day once again.

 

Thanks

[jeff]

HAH!

I've never trimmed my toolpath like that before. But you can bet I'm gonna start using this feature.

 

As mentioned above, that's the very reason I browse the forum each day.

I've learned so much.