Slowing down in the corners

[alloutmx]

if i want to slow my cutter down as i enter a corner, where would i find such an option?

[Guest]

Just asked a few days ago

 

http://www.emastercam.com/board/index.php?showtopic=73090&hl=

 

Search function is your friend

[happycat64]

if i want to slow my cutter down as i enter a corner, where would i find such an option?

i thought i just told you--what up craig

[alloutmx]

Rickayyyyyyyy...yeah well i couldnt find it, and you look busy over there running the DATRON

[Reko]

LOL... That's funny.

[FROZEN]

change at point in geo or in the machine group properties adjust feed on arc move might work

[EX-wccprogrammer]

I just add a comment inside the toolpath that says "ARC FACTOR .5" or whatever factor I want. Every arc move inside that toolpath has the specified factor applied to the feedrate automatically.

 

Works like a charm, and is very flexible.

[MotorCityMinion]

"ARC FACTOR .5"

 

Hmmm, where does this go?

[EX-wccprogrammer]

Like this:

 

Arc Factor.pdf

 

The post has been edited to assign the value to a variable, and apply that factor to all arc feedrates for that toolpath.

[MotorCityMinion]

I feel like I'm on Candid Camera. Before I asked about it, I tried it with and without the quotation marks, in the tool path comments section. Nothing changed. Post Mods...

[EX-wccprogrammer]

LOL

 

The post mods are easy to do. Here's how:

 

1. Define a variable name in the variable definition section like this:

fmt	 3 arcfactor #Reduction factor for arcs

 

2. Define a variable name for the placeholder for checking the comment:

fmt	 4 arcfactorchk #Check for FACTOR in comment

 

3. Create a string containing the words to be found in the comment:

strfactor : "FACTOR"

 

4. Inside the pcomment$ section, check for the string:

pcomment$	 #Comment from manual entry (must call pcomment2 if booleans)
 scomm$ = ucase (scomm$)
 arcfactorchk = strstr (strfactor, scomm$)

 

5. Inside the pcomment$ section, add the following:

 if arcfactorchk > 1,
	 [
	 arcfactor = scan (strfactor, scomm$)
	 scomm$ = ""
	 arcfactorchk = 0
	 ]

 

6. Inside psof$, ptlchg0$, and ptlchg$ sections, before the comment$ call:

 arcfactor = 1

 

7. Inside pcirout section, insert this:

 feed = feed * arcfactor

 

That's all there is to it..

[K2csq7]

^^^^ all the software developers are ****ing bricks after that!

Nice stuff Wcc!

[Mic6]

Yea, I guess you could do it like that

[Colin Gilchrist]

Excellent use of string functions to capture the value. I think the easier way to do it would be to use a Miscellaneous Real Number on the misc values page to enter the number directly.

 

if mr6$ <> 0, arcfactor = mr6$

 

That would save you a bunch of work, and you could add several different MR values for manipulation, without having to do use the 'scan' function...

[Oppiz]

Just asked a few days ago

 

http://www.emasterca...topic=73090&hl=

 

Search function is your friend

 

I learned a few tricks from this topic. Great!

[EX-wccprogrammer]

Excellent use of string functions to capture the value. I think the easier way to do it would be to use a Miscellaneous Real Number on the misc values page to enter the number directly.

 

if mr6$ <> 0, arcfactor = mr6$

 

That would save you a bunch of work, and you could add several different MR values for manipulation, without having to do use the 'scan' function...

 

In the early stages of my post editing, I relied on MI's and MR's to do a variety of things. I soon ran out of available features, and wanted to do more. I figured out how to achieve very cool results by typing comments and executing sections of code based on comment input. I am currently working on integrating custom probing using comments as the main driving force behind the code.

[Colin Gilchrist]

Well that is certainly impressive work.

 

Regarding probing, you should really check out the Productivity + add-on to Mastercam. It is amazing for programming probing toolpaths. We have integrated Renishaw's software into ours as a toolpath, and you can now program all your probing cycles, including using logic like GOTO labels, adjusting machine offsets, and much more.

 

It is now possible to program a contour, then a probing cycle to measure the block, and based on the measured values (stored locally on your control in variables), adjust the wear offsets and re-cut the contour. Then measure again, and repeat or move on to the next cycle.

 

In addition to the normal measurement cycles, you can write incredibly details macros and be able to backplot the motions in Mastercam. Our post department just went through a week of training from Renishaw on how to use and support their product. I was very impressed.

[EX-wccprogrammer]

I need more flexibility than a 'cycle' affords. For example, I have a 4-axis part that has opposite sides face machined at a 7 deg angle. I need to measure the distance between the corner of one side and the corner of the other side. There is no cycle that I know of that will check the distance between two theoretical intersections.

 

I prefer not to write macro code by hand, which is why I am making a post. I can program the touch points and directional vectors as a toolpath and add probing instructions as a comment inside the toolpath. This comment would include the description of what I want probed (Distance) and a variable name to store the data for later retrieval. The output code from the post will be macro commands for the probe.

 

So, this will also produce a program in which a feature can be machined, checked with a probe, adjusted and remachined if necessary.

[Colin Gilchrist]

I need more flexibility than a 'cycle' affords. For example, I have a 4-axis part that has opposite sides face machined at a 7 deg angle. I need to measure the distance between the corner of one side and the corner of the other side. There is no cycle that I know of that will check the distance between two theoretical intersections.

 

I prefer not to write macro code by hand, which is why I am making a post. I can program the touch points and directional vectors as a toolpath and add probing instructions as a comment inside the toolpath. This comment would include the description of what I want probed (Distance) and a variable name to store the data for later retrieval. The output code from the post will be macro commands for the probe.

 

So, this will also produce a program in which a feature can be machined, checked with a probe, adjusted and remachined if necessary.

 

Yes, that is exactly what the custom macro option is for. If you can dream up a way to take the measurement you want, you can write the logic in the RenMF (Renishaw's post processor), and tie it into the Probing interface. Then in Mastercam, you would select the custom cycle that you wrote, and pick the data inputs you need, directly from your part geometry. This isn't some canned cycle stuff, it goes waaaay beyond that.

 

For your needs, you would need to work with Renishaw to get the macro logic written and working, but you really can tie it all into the Mastercam interface.

 

The resulting NC code output is the Mastercam toolpaths, and all the renishaw macros and custom variables written into a single NC file.

[EX-wccprogrammer]

I was unaware of that. I will take a look at what they have going. Thanks!