setting the order of multiple profiles

[80083r]

Hi,

I have a simple 2d drawing with several profiles that I am cutting out of plywood - something we do fairly frequently for 1-off jigs and such.

I can make profile cuts in the right places, mostly, but the order that edgecam cuts the separate profiles seems totally random and wholly inefficient.

Is there any way to manually set the order that cuts are made? Not an automatic "best fit" that they always get wrong, but actually select the profile (or pocket or holes, etc).

[jasper]

Hi

1st option: Windows selecting a set of profiles:
check the closest neightbour option to optimize cuts, it may be worthwhile postioning your tool first close to the first profile you like to cut, because of the check closest neighbour the algoritm will inspect which profile is closest then cuts it, when finished it goes to the next closest uncut geometry and so on.

2nd option: Manual select by chain a set of profiles:
Doubleclick (chainselect) all profiles individually in the order you want them to be machined (leave closest neighnour unchecked now!). Now edgecam will machine in the selection order.

Hope this helps

Jasper

[80083r]

Thank you - that is the logical thing, and what I expected - but it doesn't matter what profile I select, in what order, or where I put the start/end point, it just does them in some random order (which changes from time to time). I put in a call to our reseller for tech support, but that was last week -they said they'd call me back, no luck so far.

[jasper]

that's strange, I have just doublechecked on my system (ec2009R2) and it seems to work fine, you could send me a part I try it for you

jasper

[80083r]

Here's the file I'm using - please tell me what I'm doing wrong

I've been fighting it for a while - tech support still hasn't called me back. I've tried nearest neighbour and turning it off and selecting in order. It's just lines and arcs -does that make a difference?

[jasper]

Hi,

I have looked at the part and got it to machine in the order of the selection. It seems when the helical option is checked in the depth tab, edgecam doesn't care about the order of selecting the profiles and it machines it in a "random" order. So leave the helical unchecked and it will machine in the order you selected.

Good luck

Jasper

[80083r]

Thank you very much - now I just have to play with the approach - the tool isn't centre cutting (mind you this is only mdf).

I'll have to talk to my reseller about that - I'm not able to contact Planit directly.

[jasper]

Hi,

I will also report it Planit. Good luck

Jasper

[rider23]

Looking at your drawing profile I could get the parts to machine as they were selected but made things a little quicker by joining the lines so that a profile could be selected by clicking on any part of it with the mouse. to do this I went to the design side of edgecam, went to the geometry Column and selected the continuous command, then double click on your profile line and if the profile is complete without any breaks it will all be high lighted.
The advantage of this isn't just to make selecting easier but to also check to make sure that the profile is properly drawn.
Then when you select your profiles for machining it follows the order that you select.

To get the tool to ramp into the part ,in the profile cycle there is a lead columns where you can select the direction from where the cutter is to start its approach from ,in your case a vertical approach seems best, then you can pick the angle and length of the approach.

[timf]

use a different profile cycle for each shape and you will decide the order by selection

[80083r]

That's a valid comment, and what I ended up doing. There are times when I want to change the feeds and speeds of a large number of operations like this, all at the same time.

Is there a simple way to accomplish this?

On a related note, I'm STILL waiting for a callback from tech support at my reseller. They're not very good at a) answering questions or b) calling back.

[jasper]

Originally Posted by 80083r That's a valid comment, and what I ended up doing. There are times when I want to change the feeds and speeds of a large number of operations like this, all at the same time. Is there a simple way to accomplish this? On a related note, I'm STILL waiting for a callback from tech support at my reseller. They're not very good at a) answering questions or b) calling back.

That is terrible, they should reply to you. I (reseller in Netherlands) have reported the issue to Planit. It has been logged and a dev task has been raised. I don't know when this will be fixed, this depends on improtance (= are there a lot of others reporting this). I suggest you contact them again and see what your reseller has done, best thing for them is to also report this to planit.