What's new
What's new

Edgecam and Inventor parts - 2D toolpaths

Uhrenholt

Aluminum
Joined
Jan 28, 2016
Hi,

At my place of work we use Edgecam for programming, it works great for drilling holes, but I miss the feature where you can choose a line on a solid and do toolpaths on that line.(like Mastercam)

Is there some place in some settings where I can do something about it?

The feature finder is OKAY, but like the fact that I have some more possibilities when programming...

And what about toolpath calculation time, is there anything to do about it? Running small end mills on core and a cavity, it takes waay too long time generate toolpaths. And no, I'm not using waveform for end mills under 2mm, then it would take a day to generate roughing paths. Waveform is great, but when it is single part manufacturing, we can't use 20-30 minutes looking at a frozen screen for one toolpath (if you ask me)... If we had to make 1000 pieces or more, It wouldn't bother me too much...

Cheers, Daniel
 
My first suggestion is to go download Inventor HSM Express: it's free and you can choose all your own geometry. I went through the same thing with CAMWorks for SolidWorks and now use HSMWorks.
 
We don't have inventor in the workshop, only in the design and automation department:(

I'm back to this company working, after 7 years another place. They did have Mastercam before, but suddenly someone higher up ordered Edgecam without asking the ones programming...

Well, I'm just glad that I'm not paying people sitting and looking at frozen screens...

Cheers,

Daniel
 
I bailed on Edgecam on (turn-mill) version 2013...I don't know what version you're running, and I don't know if they made any changes on this since then: Edgecam calculates an STL file after every operation to track remaining stock, and when you update/change an operation, it has to regen all those STL files. If your part has a lot of operations and you're depending on 3D remaining stock...it's going to be crunching for a while. Hope that gives you some direction...but probably best to send your file to the support guys to see if they have some suggestions.
 
I do all my "design" in rhino, and only use edgecam for toolpathing. Therefore I use a lot of wireframes for toolpath generation. Edgecams feature finder would be great if you had the time to put into it and tweak it, and were running production on similar parts and family's. But for the one off, two off mirrored parts that I do with a mix of both 2d, 2.5 and complex surfacing I found it best to generate all my 2d paths from wireframe. I've gotten to know edgecam pretty well over the past 8 years, and this way gives me complete control over what I want it to do. I always found I was left wanting more options when strictly driving off solids. You gotta have your head in the game for retracts, and leads though....(I do import the solid model for visual reference, and find edgecams "backplot" leaves no surprises as to where the tool goes).

As far as the stock creation using stl, well.....yeah its a bit "dated", but I've turned that into a positive too, and cut huge amounts of time off our big surfacing programs by using the stl stock to both rest rough, and semi finish in one go. Edgecams rest rough won't allow you to have a different offset to what you roughed with I.e. rough leaving 0.02", well if you want to rest rough using the check box you also have to use 0.02" and the amount of dumb retracts are mind numbing and unchangeable. Now I bring the roughed stock in, and rough it using a smaller tool (90% 1/2" ball) at say 0.003" and now I've combined my semi finish, and rest rough into one neat little package, using a toolpath strategy that actually cuts material and not air with a billion retracts zipping all over the place.

In you case edgecam want you to create base entities and surface curves in order to drive off them like you want to do. It's been a long time since I've used edgecam for that, but I'm pretty sure that's what you need to do. Create more geometry to drive your paths. I do it the same way only I use rhino for it, not edgecam as edgecam does not have a very good CAD interface.....
 
What are your pc specs? Maybe that has something to do with the long wait times....
I have an I7-4770 quad core @3.4GHz, 32gb RAM, and an Nvidia Quadro K2000 and sometimes Mastercam chugs if I am working with a big file.

edit: Also, Mastercam needs an Nvidia card as they don't support the AMD cards. It will work with an AMD, but not very well. Maybe edgecam plays better with one video card or another?
 
What are your pc specs? Maybe that has something to do with the long wait times....
I have an I7-4770 quad core @3.4GHz, 32gb RAM, and an Nvidia Quadro K2000 and sometimes Mastercam chugs if I am working with a big file.

edit: Also, Mastercam needs an Nvidia card as they don't support the AMD cards. It will work with an AMD, but not very well. Maybe edgecam plays better with one video card or another?

Well, I don't remember exactly what computer we have at the tool section, but I had a battle with the IT guy a little month ago about our graphic card. It's a AMD gamer card of some sort, but he kept saying that it didn't matter, it ended with me asking if he had his educating diploma by mail... No reaction on that, and no better graphic card

The computer you have is about the same I have at home, but I only have 16gb ram:-) great graphic card, the price was about half of the PC:-)

BTW. Is there a feature in this forum so I can get a note by mail when someone post in a thread I'm following? I have a hard time remember:-)

Cheers,

Daniel
 
check your output tol,both in drawing and outputting code, could be that you have it set to something like (.0001) which would cause it to generate very slow.
 
Tol is 0.01, so nothing there... We will nuke the computer next week and install everything again.

Talking Edgecam, how can I change something, so I don't get that extra file with the tool list? I have that in the start of my program, so the files just makes the folder on the PC messy...
 
First, which version of edgecam are you using? I use 2014 and 2016 and using 2D geometry is easy.

In the machining tab, click Milling Cycles -> Profile Milling. You'll have the option to use Wireframe, or Solid Geometry.

For wireframe you first need to create 2D geometry off of the solid. Go to the Features tab and click Geometry, choose Copy From Edges, and create Individual Curves.
Now simply select, box select, or chain select the edges that you want to create your 2D geometry from. By default it will create the geometry exactly on the model, so it will look like it created nothing. Simply turn off the layer for the 3D model and you'll be able to see your 2D geometry. Often it's easier to have that geometry float an inch or so above the part so you can see and select it easily. To do that when you are picking your geometry there will be options at the top of the screen, click the 2D button and enter the Z value in the level box that is at the bottom near your view selection. Now any geometry you select will be "projected" to that Z level as flat, 2D geometry.

Now simply go to Machining->Milling Cycles->Profile Milling, choose wireframe, all your desired settings, and use your 2D geometry just like you would in Mastercam.

To use solid geometry you first need to manually create a feature, not feature finder. Go to the Features Tab, Click Mill, and choose Profile_Edges. Now select the edges you want to create a feature from, then the vertexes that represent the top and bottom of the feature and finish. If you don't want to select the vertexes simply right click out of it and double click the feature after the fact to manually change the level and depth.

Now use the same Profile Milling cycle and select Solid, then select the feature you created as your geometry. Remember, the level and depth you put in the feature correspond to the level and depth in the cycle. Choosing 0 for level and 0 for depth means it will profile it from top to bottom. Putting .020 in depth means it will profile down to 0.020 from the bottom of the feature.

As for video cards, your IT guy is wrong about the AMD card. Edgecam does not work properly with anything other than Nvidia cards, and officially only Quadro cards are supported. You will run into issues picking geometry off of solids if you use an AMD card, the geometry simply wont highlight and you can't pick anything. To work around this go to the settings and turn on "Use Software Rendering Only". Keep that setting on until you buy an Nvidia card. The graphics will look crappy but you'll actually be able to work.

As for slow processing times, likely it's just a slow computer, I never have to wait more than about 5min for one toolpath to calculate, and usually that's for really fine surfacing, not something simple like roughing. There are a few things you can do to speed it up, first turn off Auto-Regenerate while you're making lots of changes, it will regenerate everything in the sequence everytime you make any change, really you just want to regenerate once at the end.

If you're going to make a change to lots of cycles in one go, turn on Batch Mode, make all the changes you need, then hit regenerate and allow it to make all the changes in one long line, go get a coffee or work on something else in the mean time.

Third, for big, complicated parts double click your sequence and turn on Background Processing. You choose a safe start position that the tool returns to between each toolpath, so that changes to one toolpath don't effect the others. Now when Edgecam is calcualting changes your screen does not freeze, and calculation happens in the background and you're free to continue working on the file and adding new toolpaths. Also make sure all your "Update Stock" commands are set to Very Small, and don't update stock if you don't have to.

Hope that helps!
 








 
Back
Top