Thread and cut pos in 9.1 for wire?

[Ronan]

Hi everyone, I just updated from MC 9 to MC 9.1 and I'm having trouble picking the thread and cut position.Every time I backplot in MC 9.1 It starts the cut at 0,0.Is this an error due to a default in one of the parameter pages.Any help will be much appreciated.

Thanks...Ronan,

[CPeast]

Create A Thread "Style" point

Create A Cut "Style" Point

 

The thread / cut points should not be on the contour geometry

 

Toolpath/Contour

Pick the thread point

Pick the chain

Pick the cut point

Click Done

 

You will notice on the

parameters page > "Origin / WCS" page the start point was inherited from the cut point you chained. If no cut point was chained you would need to set teh value of the cut point there or it will default to 0,0.

 

As you already know.

[medsourcebob]

i tried that with a 4 axis cut and it did not work

[Allan]

There is a very good document in the startmenu ,programs, mastercam >what's new in Wire 9.1.

 

It will explain all about the new features in Wire

 

HTH

[Brent Wilkerson]

I also have a problem similar to this. I've haven't had time to sort it out, so I'v been using Wire 9 instead of 9.1.

 

What I get is this. I'm doing a 4-Axis cutting with 4 skims and reverse cutting the skims. I got the new thread point and starting point firgured out. But after the first rough pass it's goes back to the thread point then to the end of the contour and then starts the skims. I can open an existing file and it's fine I can just not make a new path in a new file the same way it did in v9.

 

Here is an example of the posted code.

This is at the end of the rough and start of first skim.

 

V9 posted code...this is correct

G01X.12244Y1.2061U.07578V0.

G01X.11396Y1.21459U.07578V0.

G01X.10196Y1.21459U0.V0.

G40

G69X.86614U12W10

G62 X0

G00X.10196Y1.21459U0.V0.

G42

G01X.11396Y1.21459U.07578V0.

G01X.12244Y1.2061U.07578V0.

G01X.025Y1.10866U.07578V0.

 

V91 posted code...notice the move and back. This would cut the profile all off I just cut. Notice the bold lines of code. This is not how it was done before. I need the reverse skim cut to start where it left off, NOT go back to the contour start point and then back to the end point where it was at!

 

G01X.11396Y1.21459U.07578V0.

G00X.10196Y1.21459U0.V0.

G01X.10196Y-.02849U0.V0.

G40

G69X.86614U12W10

G62 X0

G00X.10196Y-.02849U0.V0.

G42

G00X.10196Y1.21459U0.V0.

G01X.11396Y1.21459U.07578V0.

G01X.12244Y1.2061U.07578V0.

 

It was messed up before in V9, but once you firgured it out it was ok. Now you go and change it completely, 180° different and I can't even reproduce the same program as before. I've read the "What's new" page and this is not described in it. I can upload a file of the orignal V9 part that worked and a V91 file.

 

This needs to addressed I think. If I'm doing it wrong thats fine, I just need to know where?

[chad fisher]

When i recieved 9.1 I had waited to to istall it till my new computer came in, now installed I am going to

go back to wire 9 because I am having trouble grasping this new way. Maybe in time I will get used to it, but as of now I dont have the time to play with it.

[CPeast]

Brent,

 

I have only done 2 axis work so far in 9.1 but I did notice this statement in the whats new. Just ashot in the dark.

 

If a new thread point style is used without a corresponding cut point, the wire will return to the thread point or thread distance when Auto position cut point is selected.

 

Obviously this should be after all skims, but thought might be worth looking at.

 

[ 05-01-2003, 11:31 AM: Message edited by: CPeast ]

[Brent Wilkerson]

Chad,

 

I agree totally...

 

quote:

---

If a new thread point style is used without a corresponding cut point, the wire will return to the thread point or thread distance when Auto position cut point is selected.

---

I have the Auto Start posistion unchecked. It still doesn't work. I've selected the thread and cut point I want. We are cutting an open contour and I don't actually thread and cut the wire at the machine. The wire is cutting a profile and leads in and out of the part.

 

I'm cutting an open 4-axis contour. I'm going to upload 2 files tonight from home, can't upload via FTP from work. One is the original V9 file that works. And the other is the V9.1 file. They will be in the MC9 folder in a zip file called threadproblem.zip Otherwise if anyone would like to look at it I can email the file to them.

 

I'd like to firgure this out as soon as possible.

[Brent Wilkerson]

I've upload a zip file then of threading problems I'm having. There are two files in the zip file, one has from V9 and the other has V91 in the name. The V91 one has the problem in it that I'm seeing.

 

ThreadProblem.zip File in the MC9 Directory

 

If anyone can take a look at them I'd appreciate it.

[Roger Martin from CNC Software]

Brent,

 

Check out the MC9 in the Thread_Cut_Points.ZIP

in the MC9 folder of the forum FTP site.

 

Is this the result you were looking for ?

 

I included the Thread & Cut Point (actual point entities in v9.1) in the chaining

[Brent Wilkerson]

Roger,

 

Ok how did you do that? That's what I'm trying to do. Do you have pick thread&cut points and if so how?

 

I see the 2 two chains and 2 chain points. How do you do that?

 

Thanks alot...once I figure out how to do it myself I'll thank you again!

[Oppiz]

This is how I do it. Before you go to contour.pick thread/cut,position. then place your chain points where you want them. Now go to contour, pick your chain points(thread/cut points) before your chains. I don't use "auto start position" or "thread distance" when doing it this way. This give me the results I want. It took me awhile to get the hang of it now V9.1 is a breeze.

[Brent Wilkerson]

That what I'm doing but I wants to cut back to the thread point after the rough and start of the first skim. I select reverse for the cutting method and it goes from the cut point to the thread point and then back to the cut point and reverse cuts the skim(s).

 

It's quite the pain in as*

 

I really want to figure this out so I can start using V9.1 mill and lathe so I can find more "new and improved" stuff

 

I'm sure once I figure it out how it's done it will work fine, but geez this is harder then it was before!

 

[Roger Martin from CNC Software]

Brent,

 

Sorry for dropping a sample part with no explanation.

I haven't been back to the forum 'til now.

 

You have Thread & Cut points defined, but you have not selected them.

Since you have these points ON the endpoints of what you are going to chain,

you need to be a bit careful when selecting the these points.

 

You could fix the chaining in your program using the Chain Manager.

Click on the Geometry line of your operation, right-click, select Add Chain ,then add the Thread point

Select 'Point' for the chaining method, the 'Point' to tell MC that you want

to select ONLY a 'point' entity, then drag 'n drop that point to the top of the list.

Now repeat this procedure for the Cut Point

(except you don't need to drag 'n drop this point, it's already at the end of the list.)

 

This may sound complex, but it's actually quite easy once you've played around with the Chain Manager.

 

 

BUT, (in this case) it's not a big deal to just re-chain everything...

 

This is the sequence I used when chaining everything (I rebuilt the entire operation) ->

 

Wirepaths, 4-axis (checked that the Sync Mode = Entity)

Chain, Mode, Point, Point - then select the Thread Pt.

Now Chain the lower profile.

Now Chain the upper profile.

Mode, Point, Point - then select the Cut Point.

 

Again -

The extra 'Mode', 'Point', 'Point' menu selections here are because your

Thread & Cut points are ON the endpoint positions of the profile you are going to chain.

So we need to be specific in telling MC that we want those 'point' entities,

not the endpoints of the profile. BTW, You could also do this using the Color Mask option

if your Thread and Cut Points were a different color than the adjoining entities.

 

You can make this chaining process a bit easier (a few less menu picks) by eliminating

the first and last lines of your profiles. MC is going to cut from the selected Thread Point

to the start of the profile anyway, and from the end of the profile out to the selected Cut Point.

This way, with your Thread and Cut points just 'floating out in space' you don't have to

concern yourself with telling MC that you just want to select a 'point', since there is

nothing else for MC to grab onto at these positions in space.

 

 

Also, make sure that "Thread Distance" is Un-Checked.

You're using the Thread and Cut points you've selected, so you don't want this active.

 

Roger

[Glenn Bouman]

I thought you may have had a post problem but after looking at your files, it is the lack of thread/cut points selected.

 

[ 05-06-2003, 07:20 PM: Message edited by: Glenn Bouman ]

[Brent Wilkerson]

Ok I finally got this thanks for setting me straight Roger.

I only think I don't get is this was suppose to be an improvement? I personally like the STCW dialogue box from V9 and I never had problems with multiple thread and cut points on multiple profiles.

 

Glenn,

before in V9 I'd select my thread pt at the start of my profile and the cut pt and the end of the profile. I manually draw in the lead in and lead out I want, which in my eyes is easier being I get want I want to cut faster and easier.

 

We mainly do 4-axis open contour cuts here which were easier to use with STCW but may in time I'll see the bigger picture.

 

Thanks to all who help me to see the light. I am now saved.