REDUCE FEEDRATE

[ELIAAS]

HI EVERYBODY

 

I want to know how can i reduce feedrate at corners-per each operation-is it possible?

 

 

thanks

[Robert Ouellette]

yes it is possible. you have to use the highfeed button and then you set it up to what you want to happen. you tell it the min feed you want. how much you want to reduce feed per step. set your angles to tell it what corners to use it on. little bit of trial and error at first but it is very easy to figure out. i used it alot on our waterjets too slow down in corners to let the jet catch up and cut a cleaner corner. if you need more help just ask.

 

Bob

[Chris In-House Solutions]

You can also add some logic into the post to do this, however it will slow down by a percentage of the set feed rate.

[ELIAAS]

THANK YOU

 

I did not understand enough good can explain more-

[ELIAAS]

HI

 

CAN I reduce feed rate when for example if i work with mill cutter dia 10mm-feed rate 1500mm/min- and i want that when it approach to radius 6mm-on contour-to reduce its feed rate to 300mm/min-to controll per each operation

thanks

[Chris In-House Solutions]

What version of Mastercam are you using? You can probably do a search on here for information regarding the Hi-Feed Function that Robert spoke of. Its not the simplest thing to explain through a forum however I am sure there is a lot of information about it.

 

If you want to have your post modified to do this I would recommend you contact your reseller to have them put the logic into the post.

[K2csq7]

Here is the highfeed button.

[ELIAAS]

HI

 

I USE MASTERCAM X6 MU2

[scubafan]

Be careful, I was curious myself and started playing with this high feed feature. Now everytime I try it again on the same toolpath, Mastercam crashes. In Esprit, all you have to do is check the box "corner slow down". And this high feed feature is really hard to use and makes no sense. I tried it and it didnt do anything at all to the selected toolpath. Didnt change feed, toolpath, nothing. Only thing it did change is now it crashes everytime I try it again on that toolpath. I'm going to email support about it but probably wont get a response as I have not recieved on on my last 3 submissions. I am considering pushing for a different software, Mastercam has become very unstable and alot of simple features, like corner slow down, you have to jump through hoops to use.

[Guest]

Engineering / Manufacturing Systems

Epicor Vantage Enterprise Software System

Predator System Virtual CNC-DNC Software

Neoware Data Collection Terminals

Ashlar Vellum Xenon CAD Solid Modeling

Catia & SolidWorks

Virtual Gibbs CAD/CAM Solid Modeling

Partmaker Multi Axis Lathe Programming System

 

Slumming on a Mastercam forum

[K2csq7]

Be careful

Welcome to the forum!

So, you like to scubadive?

Been thinking of getting certified, any words of wisom?

[Smit]

Also, in the tool settings of the machine group properties is a box to check for adjusting feed on an arc move. Give it the minimum arc feed and it will slow the tool down.

 

It's pretty primitive, and I really wish they'd put this inside each operation in the operations manager.

 

But it is an option.

 

When I do use it I will apply it to an operation, regenerate the operation, lock the operation, then uncheck the box so it's not applied to operations I don't want it applied to.

[EX-wccprogrammer]

This can be adressed automatically with the post processor file. The programmed feedrate can be adjusted by comparing tool radius and interpolated radius. So, whenever the cutter enters a tight corner, it is slowed down automatically. Conversely, if it is interpolating around an outside contour, feedrate is increased. This maintains constant chip load at point of contact.

[Smit]

This can be adressed automatically with the post processor file.

 

Sounds slick. Is that functionality included in the MPMaster post?

[EX-wccprogrammer]

It is in mine. Not a standard feature, though.

[Chris In-House Solutions]

Eliaas Depending on what type of work you are doing the HighFeed Function may work for you here is a brief overview of how the function works. Create you toolpath then pick your toolpath and choose the highfeed option. Choose the option at the top "roughing and finishing" Then enter your maximum and minimum feedrate. This is where it becomes tricky you need to test your machine to know what your maximum feedrate can be while going around corners and allow you to maintain your tolerances. There is also an up and down scale factor this is basically how fast your machine can accelerate and decelerate between corners and straight cuts. Setup your stock and choose Okay then in the ribbon bar choose the play button this is what actually puts the Highfeed machining into effect. A pop up will come up telling you, you have reduced your cut time by X amount of time choose yes. Upon backplotting your new toolpath you will notice there are a lot more points as shown in the graphic. This is because it adds points to adjust the feedrate while entering and exiting a corner. That's basically it in a nutshell. Its a great function, however takes some time to set it up.

[BestMastercam]

Here is the highfeed button.

 

hahahaha.....

[Zoffen]

This can be adressed automatically with the post processor file. The programmed feedrate can be adjusted by comparing tool radius and interpolated radius. So, whenever the cutter enters a tight corner, it is slowed down automatically. Conversely, if it is interpolating around an outside contour, feedrate is increased. This maintains constant chip load at point of contact.

 

How does the post know if its an inside or outside corner?