Change At Point Problem

[NeilJ]

I'm having a problem getting Change At Point to work properly. Change At Point fails if I try and doing something like the following:

 

Draw a 5" by 4" rectangle with .255 radiuses.

 

Use a 1/2" end mill to do an inside Contour toolpath.

 

Start point can be mid-point of any line.

 

I wish to mill the lines at 60 IPM and change the feedrate on each radius to 5 IPM.

 

If I start at the mid-point of a line I can get 3 of the 4 radius's to have the correct (5 IPM) feedrate.

 

Starting at the beginning of a line is the only way I can get all 4 radiuses to have the proper 5 IPM feedrate and that's not what I want to do.

 

What am I doing wrong?

[Fig sign]

What am I doing wrong?

~~~~~~~~~~~~~~~~~~~~~~~~

Dealing with idiots .

Although I know the answer ,you will never get it .

And to say truth ,never in my life I was needed to drop feed in such a drastic way .

There are better ways to deal with it .

Still you will not get this from me

:shrug:

[YoDoug®]

I don't have MCX on my home computer anymore so I can't try it but you could try breaking the side that you are selecting as your start side into two entities.

[Colin Gilchrist]

Jon,

 

I did a test and the only thing I needed to do to get it to work was break the line where I wanted to start into two pieces. There is a check box in Lead In/Out that let's you enter/exit at the midpoint in a closed contour. If you are using this it ignores one of the arc's 'change at point' info.

 

Just create the rectangle with fillets, break one of the lines, chain the contour at that start point, and use the change at point to get it to work...

 

HTH,

[OTOMMYO]

I know how, its easy

[Fig sign]

Just create the rectangle with fillets, break one of the lines, chain the contour at that start point, and use the change at point to get it to work...

~~~~~~~~~~~~~~~~~~~~~~

Colin ,may be short video ?

[Namliek_J@TheeCircle™]

How about insert a feedrate into the g-code by hand. That was hard.

[Tyler Robertson]

quote:

---

And to say truth ,never in my life I was needed to drop feed in such a drastic way .

There are better ways to deal with it .

---

]

 

I've had to do this with 6-axis waterjet on a number of occasions.

That said, what colin said should be fine. I tend to use the toolpath editor to do this, as I very rarely would change anything afterwards, and I like to review the path before I post anyway.

[Jammer™]

GTE:D

[Mike Mattera - TFM]

Iskander: What is that shadow I see on your screen image? I know what it looks like.

 

Mike Mattera

[BernieT]

Where is there a 'thank you' for the help???????????

 

 

[Fig sign]

Iskander: What is that shadow I see on your screen image? I know what it looks like.

~~~~~~~~~~~~~~~~~~~~~~~~~~~

This is to shoot those who run and pushes to pash

violently and the love and frolic .

Fot their personal safety .

 

Mick ,just say I am not an idiot !

[NeilJ]

Still having lots of problems with this and can't get it to work. Perhaps the answer to these two questions might finally help me get to the bottom of this:

 

1. When you click at the beginning of a entity where is the feedrate supposed to change?

 

2. What is the purpose of being able to put a different feedrate at each end of an entity?

[iowajim62]

quote:

---

Still having lots of problems

---

should prolly submit it as a software bug

[NeilJ]

Forgot to mention that I have broken the side I wish to start and end on into two entities and that the check box in Lead In/Out that let's you enter/exit at the midpoint in a closed contour is not checked.

[mold100]

Jon,

 

Which version and service pack are u on?

[NeilJ]

X2 MR2 SP1 (11.2.4.6)

[mold100]

Have you tried Colins method, also are you making your changes and posting to see the machines code. Also I am not sure what material you are machining but that is drastic change.

[NeilJ]

"Have you tried Colins method"

 

From what I have already posted I thought it would be clear that I have tried both Doug and Colin's suggestions.

 

"also are you making your changes and posting to see the machines code."

 

I'm using Backplot. Is there some reason Backplot won't show correctly for Change At Point that I'm not aware of?

 

I've tested Backplot by posting to compare what I have done with Change At Point and the post is the same as the Backplot.

[gcode]

Its working OK for me in X3

The toolpath feedrate is 10 ipm

I used change at point to set it to 4. at

the end of each arc and back to 10. at the

end of each line segment

This is the result

 

 

N235 ( 1/4 FLAT ENDMILL)

G00 G17 G90 G54 X9.0793 Y2.8299 W0. S2139 M03

G43 H235 Z1.6

G94 G01 Z-.04 F10.

Y2.8799

G03 X8.9793 Y2.9799 I-.1 J0.

G01 X7.2431

G03 X7.1131 Y2.8499 I0. J-.13 F4.

G01 Y.2333 F10.

G03 X7.2431 Y.1033 I.13 J0. F4.

G01 X10.7155 F10.

G03 X10.8455 Y.2333 I0. J.13 F4.

G01 Y2.8499 F10.

G03 X10.7155 Y2.9799 I-.13 J0. F4.

G01 X8.9793 F10.

G03 X8.8793 Y2.8799 I0. J-.1

G01 Y2.8299

Z.06

G00 Z.25

M05

G91 G28 Z0. W0.

G30 Y0 M5

G28 Y0.

G90

M30

[Leigh @ Kodiak]

I think I know what Jon's issue is here. I had a similar issue with "change at point", and although the way it works is not intuitive in any way, it does work.

 

When selecting the point you want to change, select at the END of the corosponding chain segment you wish to change. This will change the feed rate at the start of that segment. The feed rate for the rest of that chain will now be set to this. You will need to "change at point" on the END of the chain segment where you want your original feed rate. Follow this procedure until you are back at the start of your chain. Oh, and the process becomes even more picky if trying to use this feature on a solid chain, due mainly to solid chaining issues I see with Mastercam.

 

A pretty contrived procedure if you ask me, although I suppose such detail does have a purpose at times. Personally, I would just like the option to make the feed rate "A" when encountering any radius smaller than "r1", and feed rate "B" on any radius larger than "r2", as well as the distance away to switch to said feed rates.

[NeilJ]

gcode->This worked. The key seems to be to select only the end points of entities and make the change there. Thank you very much.

 

Could someone please point out to me where the Mastercam Help File or the Mastercam Reference Guide properly explains how to use this function.

[NeilJ]

Racerx I was writing my post to gcode and didn't see your post.

 

All I can say is I totally agree with what you posted!

 

What really made this a horror story for me was no documentation on how to properly use the Change At Point function.

 

I would love to have someone from CNC Software who writes tech manuals be interested in posting here so the Mastercam Help file and the Mastercam Reference Guide could be made a lot better.

 

Thanks so much for the help and taking the time to write what you wrote above!

 

Getting stuff like this fixed in Mastercam's documentation is important to me.

 

[ 09-04-2008, 09:45 PM: Message edited by: NeilJ ]

[mold100]

quote:

---

Could someone please point out to me where the Mastercam Help File or the Mastercam Reference Guide properly explains how to use this function.

---

Theres the point to be made this fine highly skilled forum is where its documented, for users by users. Find that in another software.

 

Although the instructional info may not be there to step by step guide in every aspect the manual would be huge. Someone has figured it. I will take the forum over a tutorial, or even video everyday. Jon, save this thread in a txt format and create a tips and tricks folder. Most of us have one filled with info from here.

 

Glad they helped you out. Bottom line thats the purpose here.

[NeilJ]

"Theres the point to be made this fine highly skilled forum is where its documented, for users by users. Find that in another software."

 

I use Mastercam. The best on-line help for Mastercam that I know of is in this forum and I've clearly said that in other places. To think that helpful and articulate users don't exist for other software and are not available on-line is not a point I'm going to argue with you.